Krrass customer support team is here to answer your questions. Ask us anything!
Hi, how can I help?
The new generation DA-Touch controls-DA66T controller offer an even higher grade of efficiency in programming, operation and control of today’s press brakes. Ease of use combined with state-of-the-art technology go hand in hand, improving productivity.
This manual describes the operation of the DELEM DA66T controller and is meant for operators who are instructed for operation of the total machine.
• This manual does not entitle you to any rights. Delem reserves the right to change this manual without prior warning.
• All rights reserved. The copyright is held by Delem. No part of this publication may be copied or reproduced without written permission from Delem BV.
The control software is updated regularly to increase performance and add new functionality.
This manual is also updated as a result of changes in the control software. The following overview shows the relation between software and manual versions.
Software version Manual version Description
V1.1 V0311 first issue V1
V1.3 V0811 update to V1.3
V1.4 V1011 update to V1.4
V1.5 V0212 update to V1.5
V2 V1212 update to V2.1
V2.2 V0613 update to V2.2
V2.3 V0913 update to V2.3
V2.4 V1213 update to V2.4
V2.5 V0714 update to V2.5
V2.6 V0115 update to V2.6
Note: This manual is valid for software version 2.6 and higher.
The control looks as follows:
The precise outfit of your control may vary.
Operation of the control is mainly done over the touchscreen. A description of the functions and available touch controls is given in the next sections of this manual, aside of the description of the specific functions.
Beside the touch controls the front of the control consists of an emergency stop, the handwheel and the start and stop buttons.
Special function keys, which can be mounted in the top panel of the control, have their specific description parallel to this user manual and will be supplied by the machine manufacturer. This
user manual focuses on the control software and related machine functions.
Front control elements
The frontpanel, beside display, consists of the following control elements:
USB connectors
At the right side of the control two USB ports are available for connection of external devices, such as memory sticks or an external keyboard / mouse.
Operation and programming modes
The DA-Touch control’s main screen looks as follows:
Depending on the navigation button which is active, the screen will differ. The above main screen will appear having the Products function active.
Just by tapping the various modes, the specific mode will be selected.
The structure of the main screen is as follows:
In the top the title panel is always shown. In this area you can find logo information, which product is loaded, the active bend, selected subdirectory and (when activated) the service row. Also machine indicators can be found here.
In the information panel all functions and visualisation related to the selected modus are displayed and can be found.
The command panel is part of the Information panel and is the location where the controls related to the Information panel can be found.
The Navigation panel is the area where all the major modes can be found. This area is always visible. The controls, large buttons with icons, can be used to directly switch from one mode to the other.
Explanation of the main modes / navigation buttons
Introduction
In order to obtain a bend program for a product, the control offers the possibility to create a product drawing and calculate a valid bend sequence for the product. With this information, a product program is generated.
This is done with the following steps:
1 Go to the Products mode in the navigation panel and start a new product by tapping New Product.
2 Enter the product properties and start to draw a 2D product profile in the Drawing mode.
3 Check the tooling, modify or make a new set-up in the Tool Setup mode.
4 Use the Bend Sequence mode to determine the bend sequence by calculating it or manually modifying it upon your own idea’s.
5 When required modify the numerical CNC program via the Program mode.
6 Tap Auto and press the Start button in order to produce the programmed product.
Preparations
Before product programming can be started, the following preparations must be made.
• The correct material properties must have been programmed in the Materials library.You can find this on the Materials page in the Settings mode.
• The correct tools must be programmed in the Tool Library. Tools are necessary to create a CNC program. You can find the libraries for the different types of tools in the Machine mode.
Create a drawing
The control offers the functionality to create a drawing of the intended product. With this drawing application, tap Drawing in the navigation panel, a 2D profile or 3D product drawing is created. At this stage, there is no calculation of bends or dimensions: any profile or drawing can be created.
The drawing method on the Touch screen control is based on:
• Sketching
• Value setting
1) Sketching
The product as well as tool shape Sketching can be done by tapping on the screen in the different directions the drawing must have. The application will follow the tapping with drawing a line between the indicated points. The last point of the design will show always a big red dot. When the drawing dot is on the screen you can hold your finger on this position and move the finger across the screen to move the connected line in another required direction or make the line length longer. This method is the so-called ‘Dragging’ facility. The length and angle value will be visible on the screen and can be adjusted to be exact or close to the requested value.
2) Value Setting
Once the product or tool is drawn in the Sketching method the exact values of line lengths and angles can be optimized by the Value setting method. Just tap 2 times on the value of the line
length or angle to change and the keyboard will pop-up. The value can be entered in 2 ways of confirmation:
• Enter function
• Enter-Next function
The Enter function will close the keyboard after entering the value. The Enter-Next function will enter the value on the line or angle to change and the keyboard will remain opened for the
next programming step.
In case the typed value is erroneous, the “undo” button right from the input field can be tapped to return to the original value or the backspace key on the keyboard to delete the last typed
character.
3) Zoom Function
By pinching the screen with two fingers simultaeously one can zoom in and out on the drawing, tool or machine visualisation. By spreading fingers the system will zoom-in, by bringing fingers nearer to each other the system will zoom-out.
4) Fit-To-Screen
In the command icons on the side of the screen you will find a Fit-To-Screen function. This can be used when the drawing size is not clear in picture. Just tap once and the complete drawing
will be sized to fit the drawing screen.
5) Panning
With simultaneous touching of two fingers and draging them over the screen (sliding in the same direction) one can pan the object in 3D view. In 2D a single finger will also enable panning.
6) Rotating
In 3D, rotating the product, tool or machine visualisation, can be done with a single finger sliding over the screern.
7) Features of the drawing tool
• Graphical design of product shapes in 2D and 3D (if available)
• Scaled sheet thickness
• Auto scaling
• Horizontal and vertical projected dimensions can be entered
• Real scale tool design
• Various machine shapes (pressbeams and tables)
• Changing of lengths and angles
• Adding or deleting of bends
• Special bend features can be applied
• Hemming bends can be programmed
• Bumping bends can be used for big radius
• Existing products can be copied, changed and stored as a new product
• Closing dimension or highest precision tolerance selection
• Connecting 2D programs for 3D-production
Determine bend sequence
When the product drawing is completed, the control offers Tool setup mode to program the exact tool set-up as it is organised on the machine. After this you can select the Bend Sequence mode to determine and simulate the required bend sequence.
In the Bend Sequence mode, the control shows the product, the machine and the tools. In this menu the bend sequence can be programmed and checked visually. When a bend sequence has been determined, the CNC program can be generated.
Bending sequence computation
• Automatic computation for minimum production time
• Interactive bend sequence determination
• Manual bend sequence determination
• Collision visualization of product with tools and machine
• Free tool and machine shape selections
• Assignments of turn times, backgauge speed etc.
• Blank length computation
• Production time indication
• Bending sequence simulation
• Programmable finger positions
Numerical program
The Program menu gives access to the numerical program and values of the active product.
There are two possibilities to create a CNC program:
• enter a numerical program, started via Products mode, tap New Program, step by step;
• generate the program from the graphical bend simulation started via the Products mode, tap New Product, via the Drawing mode. (see: Drawing mode; product drawing).
If the program is entered by hand, there is no collision check. All program values must be entered manually. The program depends on operator experience.
If the program is generated from a graphical bend sequence, the program can be visualised during production. A generated program can be edited according to operation needs.
When a drawing has been completed with a bend sequence, and the program is stored, the program is post processed and the numerical program becomes available.
The system automatically computes :
• Necessary force
• Machine adjustments such as:
• Y-axis position
• Decompression
• X-axis position
• X-axis retract
• Y-opening
• R-axes
• Z-axes
Axes positions are calculated according to the machine configuration.
The Auto menu and Manual menu, production modes
A product program can be executed via the Auto mode. In Automatic mode, a complete program can be executed bend after bend. In the Auto mode the Step mode can be selected to have each bend started separately.
The Manual mode of the control is an independent production mode. In this mode, one bend can be programmed and executed. It is typically used to test the behaviour of the bend system.More
Back-up data, external storage
Both product and tool files can be stored externally. Depending on the configuration, these files can be stored on a network or on a USB stick. This facilitates a back-up of important data and the possibility to exchange files between Delem controls.
Help text
This control is equipped with an on-line Help function. When the Help-button in the navigation panel is pressed context sensitive help will be provided.
To activate a help window for a parameter tap the Help button in the navigation panel. A pop-up window appears with information on the active parameter.
This Help window contains the same information as the Operation manual.
The help window can be used as follows:
You can scroll through the text sliding one finger in the desired direction. By tapping on the lower or upper part of the screen Previous Page / Next Page can be used to browse through the help text.
The Index function helps to jump to the table of contents. Hyperlinks in the table help to directly navigate to the desired topic.
Tap End to close the Help window.
Listbox functionality
Several parameters on the control have a limited number of possible values. When selecting such a parameter, by tapping the parameter line on the screen, the list of options will open up near the position where you tapped the line, and the desired value can be selected.
To undo the selection and the opened listbox, tapping outside the box will make it close without changing the selected parameter.
Filter, live search
In some modes a list of entities is offered (products, tools, materials, etc.). An example of such a menu is the Products mode (product selection). To search a particular product or tool, the filter function can be used. Press the command button Filter, type a part of the ID in the enter field. Automatically, the list is limited to those items that contain the typed part. Multiple search parts can be separated by <space>.
To close an open filter screen use the keyboard-close button on the right side next to the keyboard.
Navigation
Within some modes, the program screens are divided into tabs.
The tabs can easily be selected by just tapping them. When a tab is not completely visible or not visible at all, just by dragging the tab row horizontally, the desired tab can be “pulled” in sight and be selected.
Text input and editing
The cursor can be used to enter a specific value or text within an existing input. Just tap at the desired position to do so. The cursor will appear and input will be added there.E.g. in Edit notes, where multiple lines can be entered Enter is used for linefeed. Cut, Copy and Paste are offered on the keyboard for editing convenience. Undo and Redo can also be used within this editor.
The keyboard can be shown or hidden in this multiline editor using the arrow key in the lower left corner.
Typing alphanumeric characters vs. special characters
Both alphanumeric characters and special characters can be used throughout the control. A full on-screen alphanumerical keyboard will pop up when required.
When editing a field which is pure numeric, the alphanumeric characters will be “greyed-out”and only the numerical keypad can be used. For fields which enable to use alphanumerical strings, the keyboard is completely available. Special characters as ? % – can be found using the special character button on the left-lower side of the keyboard.
Special characters (like á, à, â, ã, ä, å, æ) are supported by the on screen keyboard by keeping a character (like ‘a’) pressed.
Calculator
The CNC control is providing a “desktop calculator” available for the operator.
At the top of the screen the calculator icon can be used to switch to calculator functionality.
The keyboard area provides calculator functions which can be used autonomously. Standard functions (add, subtract, multiply and devide) including percentage, square root, square and memory functions are available.
In case calculations should use parameter values as an input, and results as an output, one can switch to the calculator from the parameter entry. This will bring the parameter value to the calculator, and the result back to the input line.No cutting or pasting is necessary. Only when entering and confirming the calculated value in the parameter entry line, it will be used forward.
Network
The CNC control is equipped with a network interface. The network function offers the operators the possibility to import product files directly from the network directories or to export the finished product files to the required network directory.
Keylock function
To prevent for changes to products or programs, the keylock function offers the possibility to lock the control.
There are two levels of locking the control. Program Lock and Machine Lock.
• In Program Lock, only a product can be selected and executed in Automatic mode.
• In Machine Lock, the machine is locked and the control can not be used.
To lock a control just tap the lock symbol in the top of the screen. Depending on the code which is used, the control will Program Lock or Machine Lock. Program Lock wil show a closed lock in grey. Machine lock will show the same lock but colored (red).
Lock symbols when Program Lock is active will also appear behind parameters to show the lock is active and modification is not possible.
To unlock the control, tap the lock symbol and enter the appropriate code. After entering, the lock symbol will show it is unlocked and the lock symbols behind parameters will disappear.
Codes can be changed upon desire. The procedure to manages codes can be found in the Installation manual.
OEM function panel
Depending on machine manufacturers implementation, the upper right corner of the screen can be used for special indicators.
To access functions related to those indicators, the OEM function panel can be opened by tapping this corner of the screen.
Software versions
The version of the software in your control is displayed at the System Information tab in the Machine menu.
Example of version number:
V 1.2.3
V stands for version
V 1.x.x is the major version number
V x.2.x is the minor version number
V x.x.3 is the update version number
The major version number is increased when new major features are added to the software.
These software changes require additional introduction and could change the normal working order. The minor version number is increased when new features and enhancements are integrated which do not change the working order. The update version number solely is used for software changes when corrections are needed in the existing software version.
When a new product drawing is started a screen with general product properties appears.First these properties, general data, should be set before starting with the product drawing.
A unique name to identify a product program. The maximum length is 25 characters.
The product ID may contain letters and numbers as available on the keyboard.
A name or description of this program. The maximum length is 25 characters. The
product description may contain letters and numbers.
If an existing product ID is entered, a warning appears that this product already exists. You are
asked whether to overwrite that existing product with the new product or not. If you choose ‘yes’, the existing product is erased. If you choose ‘no’, you must enter a new ID.
Thickness of the sheet.
Selection of the material type of the sheet. The control contains 4 pre-programmed materials. See Settings to program materials. Press the required material to select it as active.
The Z-length of the sheet.
Determine the use of the outside (A) or the inside (B) dimensions in the product drawing when new sides or surfaces are added. The figure below shows the definition of both the dimensions. By default this parameter has the value of the Settings mode parameter Default Dimensions.
The product radius is recalculated after selecting the tools in the tool setup, because the chosen tooling influences the resulting radius. By deafult this setting is ‘use calculated’.
With this parameter one can overrule and select ‘use programmed’; in that case the product radius will not be recalculated and used as programmed.
To change the active directory select Change Directory. The current product is automatically copied to the new directory.
Add Notes
When Edit Notes has been pressed, a new window appears in which you can edit the text about the current product. The possible characters are displayed on the keyboard.
To attach a PDF file to the note tap Attach PDF. Via the directory browser a PDF file can be selected and will be incorporated in the product file.
When solely a PDF file is attached without a textual note, the PDF will be shown instantaneously when the user presses the Notes indicator in Auto mode.
After entering the general product data the drawing screen appears.
In the upper information row you will find the information about product ID, product description, inside/outside dimensions selection and actual product directory.
Now you can create the profile of the product. It is possible by using your fingers to tap and create quickly the product in ‘sketch’ mode. After that the real product dimensions and corresponding values can be entered by using the keyboard.
It is also possible to directly enter the angle of the bend followed by the length of that side by using the keyboard and the Enter button. The properties are prompted in the input bar of the screen on the keyboard panel. This procedure continues until the product has the desired profile.
The product data can be changed by selecting Product Properties. The properties of the product angles and lines can be changed by selecting Properties.
The currently active element (line or angle) is highlighted. In a product drawing you can program up to a maximum of 99 bends per product (graphical programming).
When the product drawing is finished it is possible to navigate to the next step in the programming process; to determine first the Tool Setup and after the Bend Sequence.
Introduction
When the cursor is on one of the product lines it is possible to change the properties of that line by selecting Properties.
Inside the window with line properties, the following projection properties can be programmed:
The horizontal distance a line must measure, regardless of its angle value.
The vertical distance a line must measure, regardless of its angle value.
The projection function is a useful aid for drawing diagonal lines between points without having to compute the precise side length. When a line is selected, simply enter a horizontal or vertical projection distance and press Enter. The required line length is computed and applied to the selected segment.
It will be noted on the screen if projection is not possible.
Precision selection
When the drawing cursor is on a line segment, you can select the level of precision for this line. Enter the properties and go to the parameter Precision.
Select the level of precision for a line.
Normal: Achieve normal accuracy for this segment.
High: At bend sequence computation the back gauge stop position will be chosen to get the highest possible precision for this line interval.
Closing dimension: At bend sequence computation the back gauge stop position will be chosen to get the resulting tolerances in this line interval.
Example:
Line interval marked with the open circle should be, if possible, directly placed between back stop and the centre of the die.
Specifying line intervals with high precision and closing dimensions may result in longer production time.
The precision parameter will have priority over the “front extend ratio”, if that is set to “comply if possible”.
Air bend
Drawing a product graphically is simply programming the line length, angle value, next line length, etc. till the product has its required shape. The bends in the product have their standard or specific properties. The bend properties can be set by selecting the bend and selecting Properties.
With the bend type it can be determined what kind of bending process is required.
Options are:
• Air bend as normal bend with a defined angle and preferred radius.
• Bumping as bend process to realise a large radius in different steps of airbending.
• Hem bend as bend process including the pre-bend (a standard air bend with a sharp angle) and hemming action with help of a special hemming tool.
The angle value to bend.
The intended radius which is programmed. As initial value the programmed product thickness is used. This radius can also be a large radius requiring large radius tools.
The resulting radius as computed from the control settings. Amongst others the resulting radius is depending on the used tools in the bending process
A large radius is meant to be bent with a special radius punch with large radius. If such a punch is not available, the bumping method can be selected. The radius value may not exceed the length of any adjacent sides. For the definition of the line lengths to be programmed in the part connected to a radius bend, see figure below.
Lengths L1 and L2 must be equal or bigger than the radius R.
It is also possible to create a bend by placing the cursor on the flange end where the bend is required and select Properties. In this way the pop-up window will appear with an extra
parameter to fill-out.
Large radius: Bumping
If a tool with large radius is not available, the bumping method can be chosen. With this method, a large radius in a product is obtained by a series of slight bends in succession.
First you can choose the Angle Definition. The available definitions are:
• The default angle is the angle which could be programmed as standard.
• The central angle is the supplement of the default angle (i.e. 180 degrees – default angle).
To apply the bumping method, the following parameters must be programmed:
The supplement of the angle value to bend.
The intended radius which is programmed. As initial value the programmed product thickness is used.
The number of segments in which the radius will be divided. The number of bends in this radius is the number of segments plus 1.
The more segments you select, the more bends will be used to create the programmed radius within a smaller tolerance. With a high number of segments you will need a smaller V-die opening to be able to bend in a proper way.
When a product has a radius bend, the segment size is computed from the number of segments, which has been defined by the user. Standard the first and last segment are calculated half the size of the mid segments to obtain a better result. However, it can be a problem selecting a die suitable to bend these small segments. Therefore the control can calculate an equal size for all segments. This can be defined with this parameter.
When Enabled all segments will have an equal size.
When Disabled the calculation is including half size segments. If in this case a problem with the size of the V die is detected in the bend sequence determination, the user is asked whether or not to select a re-calculation with equally sized segments.
When you must program such a bend, first program a standard angle with adjacent sides.
Then put the cursor back on the angle, tap the function Properties and select Bumping as Bend Type. You will be prompted to program the radius, the number of segments and if you like to have equal bumping segments or not. After programming these parameters the radius is drawn in the product and a message will appear on the screen with information about the smallest calculated segment length. The smallest segment length has consequences for the selection of the die.
Hem bends
When creating the required profile of the product with a hem bend it is possible to first prepare a flange with a prebend angle, place the cursor on the bend and select Properties. The bend
properties can be programmed in the pop-up window.
It is also possible to create a hem bend by placing the cursor on the flange end where the hem bend is required and select properties. In this way the pop-up window will appear with an extra
parameter to fill-out.
The required angle of the pre-bend, normally a sharp angle. The angle can be set uponthe best practical value, the default value is 30 degrees.
The hem bend can be made with a certain opening distance between the 2 flanges. The hem opening value will be used calculating the beam position in the hemming process.By default this parameter has the value of the Settings mode parameter Default Hem Opening.
The length of the flange to hem.
With the marker function a specific surface or bendline can be marked improving the recognition specific of sides and bendlines.
One can select and point at a specific point in the product to place the marker. A cylindrical “label” will be placed at the point of insertion. The marker can be moved to a new position by setting the marker on a new position.
This marker will be shown in Automatic mode.
The top/bottom colors can be swapped if this would suite the situation better.
Remove the marker from the product.
When the function Tool Setup has been activated, the screen shows a front view of the machine set-up in the upper half of the screen. In the lower half of the screen, the tool data is displayed. In this screen, the placement of tools in the machine can be programmed.
In the front view, the following machine elements are shown, from top to bottom:
• Machine upper side (pressing beam)
• Adapter for punch (if an adapter is programmed)
• Punch
• Die
• Machine lower side (table).
The machine parts have already been pre-selected in the Machine mode. Normally these parts will not change. Whether an adapter can be programmed depends on the parameter Enable Adapters in the same Machine mode.
When starting a new tool configuration, the machine opening is empty.
Select Add to add a tool to the configuration; punch, die or adapter (if enabled).
When a tool has been chosen (e.g. a punch), it is placed in the machine with maximum available length.
After a tool is placed, the tool ID can be changed by selecting the Punch ID in the screen and tapping on the List view.
If only a part of the tool ID is typed, the control automatically offers a list of tools with the typed characters. This is a filtering function. By tapping Advise from this screen a limited selection from the available tools will be made and displayed.
The criteria for the selection are:
• Product radius; the selected tool must result in a product radius close to the preferred
radius. The resulting radius must be in the range of the preferred radius +/- 50%.
• The necessary bending force should not exceed the resistance of the tools.
• The angle of the tools should be equal to or smaller than the required product angle.
• The bend method should match. For example, hemming tools are selected when the product contains hem bends.
The full list can be displayed by tapping Show All.
Multi-V, die feature preselect
In case of a Multi-V die, i.e. a die with more than one V- or U-opening, a specific V- or Uopening of the Multi-V die can be selected or the Multi-V die (with V = *) can be selected. If a
specific V- or U-opening is selected, this opening is used by the bend sequence calculation; if the Multi-V die (with V = *) is selected, the control will use the opening which will result in a product radius as close as possible to the programmed product radius.
If during the bend sequence calculation another V- or U-opening is selected, this new opening
is used by the control for the remaining bends (which are not in the bend sequence yet).
Vario-V, selecting and setting
In case of a Vario-V die, i.e. a die with a variable V- or U-opening (only available if a Vario-V system is present), the selection of the die is equal to any other die. When the Vario-V is selected the V-value is not programmed yet. From here one can choose to continue and make a bend sequence. The control will use the most suitable V-value, taking the available Vario-V positions into account.
In case a desired V-value is programmed, the control will use this programmed value in the bend sequence calculation.
When the Vario-V die system is using discrete positions, only values from the available positions will be possible. When programming differently, the nearest available value will be used.
In the Bend sequence mode the selected V-opening (Multi-V) or V-value (Vario-V) can be modified. Using Modify, Shift Die, the selected V-opening or V-value is shown and can be modified by tapping on it. In Program mode the Die positioning function offers similar functionality.
Positioning or repositioning
To change length and position of a tool, move the cursor to the appropriate field, type a new value and press ENTER. When the length and position are changed, the tool is ready.Tools can be selected by tapping them, their position can also be changed by dragging them to the desired position.
The repositioning of tools by dragging is enhanced with a feature to enable accurate positioning.
When, during dragging, the finger is moved downward, the positioning speed is decreased. The further the finger is moved downward, the slower and more accurate the positioning can be done.
When dragging tools, or tool stations, the snapping function will assist in aligning the upper tool with the lower tool at left or right, or the tools or toolstations with the middle of the machine. At the time tools are within the snapping zone, a red line will appear indicating that release will help positioning towards the indicated edge or position.
After the punch is finished, a die with the default ID, with the same length and position as the prepared punch is put below the punch.
The tool set-up can be modified with the available functions or by changing a value in the list view. Punches and dies can be added or deleted, the existing tools can be moved to a different position, their length can be modified, the orientation can be changed (i.e. the tool can be turned around) and heel types can be changed.
Delete config
The existing configuration is deleted and a new tool configuration can be started.
Add
Add a new tool to the tool configuration. When pressed, some new functions are offered to choose the tool: punch, die or adapter (if enabled).
Delete
Delete the currently selected tool.
When using segmented tools, from which desired sized tools can be composed, the control can support this and can help to generate the appropriate segmentation.
In below paragraph the functionality for segmentation is explained, including the use of the three views on the tool setup. Next to the Tool Setup screen the ability to have segmentation features available is depending on the programmed segments for each tool. This programming can be done in Machine mode under the Punches and Bottom dies libraries.
More on programming of segments in the Tool library can be found at the end of this paragraph.
From within the Tool Setup screen there are three available view modes. With the selection buttons on the left side of the machine front view following
.
After the proces of setting up the desired tools for the products to be made, the Bend Sequence mode can calculate the most efficient bend sequence.
Upon desire the tools can be segmented, helping in the selection of the segments creating the correct tool length.
The tool segmentation function automatically calculates the required segmentation and uses the assignments “maximum inter tool distance” and upon choice the “tool length tolerance” for finding the best solution.
Tool view
For the segmentation of tools one can press the tool segmentation function in Toolview.
The system will, based on the programmed segment lengths and number of available segments, calculate the segmentation for that specific tool. This, taking all stations using the
same tool into account (tool segments must have been programmed in the specific tools).After starting the function, the found results are shown and the optimisation proces results can be followed. When an exact match has been found the indicator will turn green (later the color of the tool symbol is colored similarly).When a non-exact but valid length is found, taking the assignments into account, the indicator will turn yellow. This can mean that either the inter tool distance or the tool length tolerance has been used. Also it can mean that, given the fact that it is a 2D product, the tool is longer than desired. The results are shown in an information message shown.
When the result of the automatic calulation is that there is no valid segmention possible, the indicator will turn red. No segmentation will be applied.
The calculation proces can be interrupted with Cancel, or Stop accepting the current achieved optimisation.
To merge a segmented tool to a non-segmented tool, the Merge segments button can be used. When changing the properties (e.g. length) of a segmented tool, it will automatically merge into a non-segmented tool.
Assignments
The assigments used during the segmentation calculation can be found by tapping the Assignments button.
The following assigments are available:
Max inter segment distance
The distance allowed in between segments.
Use tool length tolerance
To enable this tolerance for the allowed segmentation deviation.
When switching to Segmentation view, the segments of the tools will be shown, both in the graphical visualisation and in the list below.
Only the segments from the selected tool are shown. The individual segments can be moved and changed, and the list shows the division of segments of which the tool can be build from.
Segments can be changed within the segmentation view. The available segments in stock are not taken into account at that time. With a renewed segmentation this can be verified.
When changing tool length or type, segmentation will be lost, and need to be generated again.
Segments in the tool library
To enable the use of segments, and the calculation of segmentation based on the available segments, one needs to fill out the library. This can be done in the tool programming, to be found in Machine mode, under Punches or Bottom dies in the tool properties.
In every tool, the segment’s length, the optional heel shape and the available amount of segments can be programmed on the Segmentation tab.
The third Tool Setup view is the Station view. In Station view the complete toolstations are highlighted when selected, and can be repositioned by programming an alternate position or dragging to the desired new position in the machine.
A toolstation is automatically defined when there is an overlap from punches with dies. This, meaning that a toolstation is considered a station when e.g. there is an exact position of punch
and die opposite of each other. When there is a shifted position but still overlap in between punch and die, this is still considered a tool station. Even when two punches are opposite of a single die, which can be usefull bending constrained bends, this is considered a toolstation.
These stations can be repositioned without losing their relative positioning.
Station view is not changing anything to the tool details
When a tool configuration is available, the bend simulation can be started to determine a bend sequence for the active product. The bend sequence determination is started by tapping the
navigation button Bend Sequence.
The bendsequence determination can be realised by automatic calculation starting with the bent product. It is also possible determining the sequence manually starting with the flat product, not using the automatic calculation.
In the bendsequence screen the product appears between the tools in a possible last bend position. When starting the simulation, the product is shown in its final state. In order to obtain a bend sequence, the product must be unfolded from the last bend to the first. This can bedone with the available function keys.
When it is prefered to start with a unfolded product to manually chose the bendsequence, this can be chosen under the command button Bend Sequence.
Functions
Unbend the currently shown bend or start searching for the next feasible bend to unfold.
Bend the product in the simulation screen or switch to the next bend step.
Shift the product manually (if product is bent) or shift the gauge manually (if product is unbent).
Manual selection of a bend line. Additional possibility to determine the bend sequence.
Compute a valid bend sequence. During the computation the bend sequence computation can be cancelled or stopped;
• Cancel is shown when no valid bend sequence has been computed yet.
• Stop is shown when a valid bend sequence has been computed already. This could be the not optimum in production time.
Open a screen with assignments, parameters for the bend sequence computation.
To start a new bendsequence, to reload the original bendsequence or to save a complete bend sequence. These functions can be found under the bend sequence command button.
+New
Start a new bend sequence, any existing sequence is removed. This is for automatic computed bend sequences.
+New Flat
Start a new bend sequence from a flat sheet. This is for manual determined bend sequences.
+Reload
Restore an existing bend sequence from disk, but disregard any related CNC program. This is also including corrections.
After a bendsequence has been calculated or determined, the Save and Save as can also be found in this menu.
+Save
Save a bendsequence will save the resulting CNC program on disk. The resulting CNC
program contains all necessary axis positions and tool numbers. This command can only be
executed when a complete bend sequence has been determined.
+Save as
Save as can be used to save the current product and its bendsequence under an alternative name. This enables an easy way to make product differentiations (variants).
When the bendsequence screen is left, the product will automatically be saved. If there are changes made, and save is not used, this will be prompted on the screen.
Show bendsequence
To show a mosaic screen with a step-by-step graphical overview of the bend sequence.
The bend sequence can also be viewed and determined in a 3D view. This can be achieved via the view mode selection.
View select
Within the bendsequence screen views can be switched upon required choice.
The view functions are located oposite of the command buttons in the main screen
View functions
Bend selector
Within the bendsequence screen bends can be selected and navigated thru with the bend selector. In the top of the screen the number of bends is indicated with preliminary bend selectors. After completing the bend sequence, these are all colored, active and show a turn indicator.
From then bends can be tapped to easily to select the desired bend data. In the bend selector the turn indicator will be displayed showing green, yellow or red colors to indicate the level of
complying the assignments of the bend sequence.
In order to generate a CNC-program the bend sequence must be known. There are two ways to achieve this:
• Press the function key Compute. The control will automatically compute the quickest possible bend sequence for this product.
• Press the function key Unbend repeatedly, until the product is completely unbent.
When the product is completely unbent, press the function Bend sequence and Save to generate and save the CNC-program.
It is possible that no bend sequence has been found for various reasons:
• The installed tools are not correct. Return to the tool configuration menu to change the tool configuration.
• The assignments are incorrect. Return to the assignments menu to modify the assignments.
• A collision has been detected during unbending. It is possible to manually adjust the bend sequence with the available functions. This is explained in the following sections.
Normally the control proposes the next (un)bend in a sequence. This is computed by the control depending on the programmed assignments and of course the product shape and applied tools. For various reasons it can be necessary to choose another bend line for the bend sequence. The bend sequence can be changed/determined through the function Manual Selection. When the function Manual Selection has been choosen, a new window is opened.
Functions
Unbend the currently shown bend or start searching for the next feasible bend to unfold.
Bend the product in the simulation screen or switch to the next bend step
Shift the product to the front.
Shift the product to the back.
Turn the product between the tools (back to front).
Leave the current screen without saving changes.
Save the changes and leave the current screen.
Shift product
In the bend simulation menu, the control computes the next possible bend to unbend. The
product is placed between the tools, where there is no collision with the tools or the machine.
In case you want to shift the product under the tool set (which is mounted), you can move the
product by selecting the function Shift product. A new window appears.
Jump Left
Move the product to another toolset combination in the left direction.
Jump Right
Move the product to another toolset combination in the right direction.
Shift Left
Shift product to the left within the same toolset. The step size is displayed at the command line prompt and can be changed.
Shift Right
Shift product to the right within the same toolset. The step size is displayed at the command line prompt and can be changed.
Show
Select a possible view of the simulation:
• product/tools
• all
Cancel
Leave the current screen without saving changes.
Accept
Save the changes and leave the current screen.
Shift gauge
The control automatically computes at each bend the X axes, R axes and Z axes positions.It takes into account the values of the option assignments and searches for a solution without
collision of the fingers with the product. In order to be able to choose alternative positions, you can move the fingers manually.
When the product is unbent, select Shift Gauge. A pop up window displays the backgauge fingers with one finger highlighted.
The fingers can be moved by means of the different available functions.
Select the finger to move.
Position the finger around the corner of the contact surface to fixate the product both in Xdirection and Z-direction; this is only possible on a machine with special fingers that have the pinching possibility. Also the control should be equipped with this option.
Move the selected finger to another side of the product behind the machine. In the example there are two possible finger positions to choose.
This way is only possible and will only be accepted if the required axes are enabled in the control (like X1 and X2).
Lay On Finger
Toggle between lay product on selected finger or not. This option is only selectable in case you have R-axes in your machine.
Shift Left
Shift the selected finger to the left. The step size is displayed at the command line prompt and can be changed.
Shift Right
Shift the selected finger to the right. The step size is displayed at the command line prompt and can be changed.
Cancel
Leave the current screen without saving changes.
Accept
Save the changes and leave the current screen.
Introduction
The Assignments are parameters with which the bend sequence computation is controlled.
The assignments screen is opened from the tool configuration screen with the function key Assignm.
Automatic bend sequence computation works with several conditions in order to find an optimum between a minimum production time, handling possibilities without product/machine and product/tool collision.
In order to find one of the optimums you must program several computation parameters with which the bend sequence can be computed. Some of these parameters are machine-related and some are related to product accuracy, handling possibilities and turn times.
Functions
Load default assignment settings. It is possible to determine a set of assignments which have the most optimal values for your situation. This set can be stored by tapping Save As Default.
While programming another product you can recall this previous fixed set by loading the values via Load Defaults.
Save the current settings as default assignments settings.
Leave the current screen without saving changes.
Save the changes and leave the current screen.
Optimisation degree
Range 1-5.
The number of alternatives to be computed for each bend must be entered here.
The higher this number the more alternatives are to be examined by the control, so the longer the computing time will be:
1 – lowest optimisation, fastest computation
2 – low optimisation, fast computation
3 – medium optimisation, medium computation
4 – high optimisation, slow computation
5 – highest optimisation, slowest computation
Front extend ratio
Range 0.01 – 1.0.
This is the ratio of the minimum allowable length of your product which extends in front of the press to the total blank length of the product. You must have a minimum length of your product in front of the press to be able to handle the product.
Front extend ratio accept
Comply If Possible: This means that when possible the computer tries to comply to the front extend ratio and only when this will result in no solutions to be found it will accept that the length in front is smaller than the specified ratio.
Comply Always: The computer will always comply to the front extend ratio. This may result in no solutions to be found.
Radius factor
Range 0.1 – 2.0.
The computed radius of a bend is multiplied by this factor for correction purposes. This correction affects the X-axis position and the computed blank length. The initial value of RF is 1.
The control computes the X-axis position necessary to obtain L=100 as shown in the figure below. The accuracy of the length L is dependent on the material parameters like thickness, strength and kind of material. In order to have a correction possibility with the radius factor RF you can optimise this computation.
Tool length tolerance
The tool length may be shorter than the length of the bendline.
The maximum allowed difference between the tool length and bend length can be programmed here. Tool length tolerance may influence your bend sequence: if the length of a tool is shorter than the tolerance permits, it will not be accepted for a bend.
See figure below in which the Punch length has been indicated by PL and the bending length by BL. The tolerance value is the difference between PL and BL.
Minimum Y opening
During postprocessing of the programmed product, the control always computes an optimal opening of the pressbeam to handle your product. Here you can program a minimum required opening. The programmed value is the distance above the speed change point (Mute).
Assignments – Backgauge possibilities
Backstop against sharp angle allowed
Specify if backstop may be placed against an angle smaller than 90°.
• No = not allowed
• Yes = allowed
Backstop-die, intermediate bend
Set to allow if there may be a bend between the die and backstop.
Selection possibilities:
• Permitted
• If unavoidable permitted: if it results that no solutions are to be found, than it is permitted
• Prohibited: never allowed.
Edge tolerance
In case backstop is against flat sheet an angle tolerance is allowed (deviation from horizontal). To be programmed in degrees of tolerance (0 – 90° input).
90 degree tolerance
The maximum allowed deviation from vertical (90°), when the backgauge is against a bent angle which is not 90°.
Lay-on backstop limit
This parameter is useful in case the press brake has been equipped with backgauge fingers on a moving R-axis, having a so-called “lay-on” construction.
When the length of the sheet at the backside of the machine is greater than this limit, the X-axis and R-axis positions will be corrected automatically so the sheet will rest on the backgauge finger. This is only possible if an automatic R-axis is enabled.
When the function Show Bend Sequence has been pressed, a graphical overview of the bendsequence is shown.
This option can be called at any time after the first unbend has been made. The graphical overview displays the determined bends as well as the not yet determined bends (question
mark sign).
Each image in the overview can separately be enlarged or reduced with the available functions. The images can also be rotated by finger movement.
To edit an existing CNC program, select a product in the Products overview and select the navigation button Program. When starting a new program, select New Program and after giving in the main product properties, the system will automatically switch to Program. In both cases, a screen as shown above should appear. Programming and changing data is done in the same way for both modes.
To edit an existing CNC program, select a product in the Products overview and select the navigation button Program. When starting a new program, select New Program and after giving in the main product properties, the system will automatically switch to Program.
In both cases, a screen as shown above should appear. Programming and changing data is done in the same way for both modes.
The main screen shows the existing numerical program or, when starting a new program, the first to be programmed bend.
To change the main product properties tap Product Properties. These parameters of the program are the same for every bending of the program (main data of program).
Functions
Copy the current product. When pressed, you must enter a new product ID for the copyprogram.
Choose another location (directory) on the local disk to store the current product. The product is automatically copied to the new location.
Opens a window enabling viewing and editing of notes about the current product. See more on Edit Notes further in this paragraph.
Parameter explanation
A unique name to identify a product program. The maximum length is 25 characters. The product ID may contain letters and numbers.
A number or description of this program. The maximum length is 25 characters. The product description may contain letters and numbers.
Selection of the programming mode for the Y-axis.
0 = absolute: program the absolute Y-axis position for a bend.
1 = α: program the angle to bend. The required Y-axis position is computed.
Depending on this parameter, either the parameter Angle or the parameter BendPosition will appear in a bend step.
Thickness
Thickness of the sheet.
Material
Selection of one of the programmed materials, which are used to calculate the bending depths. The control contains 6 pre-programmed materials. In total, 99 materials can be programmed on the control. The materials can be programmed on the Materials page in the Settings mode.
Blank length
The required length of the original sheet from which the product is bent. If the program has been processed from a 2D drawing, this value has been calculated.
Connect
The parameter “connect” is to have a possibility to connect certain programs to one another. This option can be used to produce 3-dimensional products out of two programs.
The main screen shows the available bends and from this main screen, from every available bend, specific paremeters can be viewed and edited.
The bend selector in the top of the screen can be used to navigate thru the bends. The indicated bends can be tapped to easily select the desired bend data.
Product Properties
Opens a new window, in which product properties, effective for all bends, are shown and can be editted.
Opens a window in which axes positions in relation to finger positions can be programmed.
Opens a new window, in which all bends are shown in a table.
Opens a window enabling viewing and editing of notes about the current product.
See more on these functions further in this paragraph.
The parameters of every bend are listed on one page and can be scrolled thru. Below the specific bend paramaters are explained.
The product ID and product description are displayed in the top row on the screen.
Tools
The name (ID) of the selected punch. Tap to modify or select from the punch library.
The name (ID) of the selected die. Tap to modify or select from the die library.
The name (ID) of the selected punch adapter. Tap to modify or select from the punch adapter library. Whether an adapter can be programmed depends on the parameter Use punch adapter in the Machine mode.
The name (ID) of the selected die adapter. Tap to modify or select from the die adapter library. Whether an adapter can be programmed depends on the parameter Use die
adapter in the Machine mode.
Program the desired tool ID or press the tool to get an overview of the available tools in the library. Press the function Turn Punch or Turn Die to change the orientation of the tool (i.e. to turn the tool around).
Turn around the applied tool (back to front). Only available if the cursor is placed on a tool parameter.
Bend parameters
Select the required bending method. The control supports 4 methods:
Air bend
Bottoming
Hemming
Hemming & bottoming
Handling
The sheet is bent to the programmed angle by bringing the punch to the required depth.
The control calculates the required Y-axis position to obtain the programmed angle.
1) Air bend
2) Bottoming
The sheet is bent by pressing the sheet between the punch and the die. The control assumes the bottom of the die as required Yaxis position.
3) Hemming
The sheet is folded in two. This is possible after the sheet has been bent into a sharp
angle in a previous bend. The control calculates the precise Y-axis position for this action: the surface of the die plus twice the sheet thickness.Y-axis positioning can be adjusted by programming a ‘hem opening’.
4) Hemming &Bottoming
The same as hemming, but now the control assumes the top of the die as required Y-axis position. The folded sheet is pressing between punch and die.
5) Handling
No movement of the Y-axis, so the current program step becomes a non-bending step.Only the backgauge axes will position according to the programmed values, e.g. in order to enable handling of the product. An external step change (C-input) is required.
Note 1:
The hemming bends are shown here with a special hemming punch, but this is not required.
Note 2:
When bottoming operation is selected, the end of bend position of the Y-axis beam depends on the working force. If however the force is sufficient for the beam to go to the calculated Yaxis end of bend position, the beam stroke will be limited by the position value.
Bending length
Length of the sheet between tools.
Angle
The required angle of this bend. This parameter only appears if angle programming is selected with the parameter ‘Angle sel.’ and the bend method is an air bend.
Hem opening
The hem bend can be made with a certain opening distance between the 2 flanges. The hem opening value will be used calculating the beam position in the hemming process.
By default this parameter has the value of the Settings mode parameter Default Hem Opening.
Bend position
The required Y-axis position for this bend. This parameter only appears if absolute
programming is selected with the parameter ‘Angle sel.’ This parameter also appears if
the bend method is bottoming and/or hemming.
Opening
This parameter results in a certain gap opening between the punch and the die after thebend. A positive value is the gap opening above Mute, a negative value below Mute.
When you want to limit the handling time of the product you can program a small positive or a negative value.
Auxiliary axis
The position of the selected axis.
When a negative value is programmed for an X-axis this value is interpreted as a relative value. This value is subtracted from the actual X-axis position. Therefore this
parameter can also be used as a chaining measure.
Retract
Retract distance of the selected axis in the current bend. The “backgauge retract” is started when the beam is pinching the sheet.
Axis speeds
Speed of the selected axis in the current bend. Speed can be programmed in a percentage of the maximum possible speed.
Edit notes
It is possible to add a note to your product, in order to store comment or background information about the current product. It is also possible to add a note to each bend.
The note is a simple text field, it has no influence on product values or bend sequencecal culations.
To attach a PDF file to the note tap Attach PDF. Via the directory browser a PDF file can be selected and will be incorporated in the product file.
When solely a PDF file is attached without a textual note, the PDF will be shown instantaneously when the user presses the Notes indicator in Auto mode.
Gauge function
The function key Gauge Func opens the gauge functions window. In this window several backgauge related parameters can be programmed. These parameters serve to program the desired finger positions for a certain bend. The necessary axis positions that are necessary for this bend are calculated from the programmed finger positions.
The required angle of the backgauge fingers for angular positioning of the backgauge.
The side length of the product to be used for the backgauge positioning (Z-positioning).
The value in X-direction of the finger position for the sheet. This value can manually be adjusted in this window, if required.
The value in R-direction of the finger position of the sheet. This value can manually be adjusted in this window, if required.
The value in Z-direction of the finger position of the sheet. This value can manually be adjusted in this window, if required.
With this parameter you can program another finger position for this specific bend. The finger position you can program depends on the back gauge possibilities. Back gauge
dimensions are programmed in the Machine mode.
• Lay-on = 0: no lay on (default)
Other possibilities are:
• Lay-on = 1: lay on first level
• Lay-on = 2: lay on second level
• Lay-on = 3: lay on third level
When setting this parameter to off, the finger is parked. When a finger is parked, the finger is positioned at its minimum or maximum Z-position, depending on the finger
being the leftmost or rightmost active finger.
Only available when more than 2 fingers are present.
When you program another Lay-on the axis positions change, but the gauge position for the sheet does not change. This means that the previous two parameters R and X remain the same. See also example below.
With Accept you leave the window and the new values have been saved. If you press Cancel you leave the window without changes.
When you have changed Lay-on then the axes positions in X- and R-direction have been changed. The new values depend on the dimensions of the back gauge finger which you have programmed in the Machine mode. When you have changed the values of R and X, then these changes are also included.
Auxiliary functions of the bending can be programmed scrolling down the bend parameters page.
Mute
Sequence point at which the Y-axis is switched from fast closing speed to pressing speed. The value programmed here is the distance of the mute point above the sheet.
By default, the mute value from the programmed die is used. Whether or not this parameter is present depends on machine settings.
Parallelism
Difference of left- and right hand side cylinder (Y1 and Y2). When positive, right hand side lower. When negative, right hand side higher. The programmed value is active below the clamping point.
Repetition
0 = bending is skipped
1 through 99 = the number of times this bending will be repeated.
Wait for retract
In case of a retract, let the Y-axis wait until the retract is finished, yes or no.
No: the retract is started when the Y-axis passes the clamping point, the Y-axis does not stop.
Yes: when the Y-axis reaches the clamping point, the Y-axis is stopped and the retract is started. When the retract is completed, the Y-axis moves on.
Step change code
Programmable parameter which determines when the parameter values for the next bending will be active. The following settings are possible:
0 = ER: Bending number change (step change) at end of decompression (next bend parameters active).
1 = MUTE: Step change at muting position when the beam moves in opening direction.
2 = UDP: Step change at upper dead point.
3 = UDP STOP: Step change at upper dead point without movement of any axis and the control goes to “stop”.
4 = EXTERNAL: Step change if C-input signal becomes active, without movement of the
beam. When you still have a beam movement there will be no retract function of the back gauge performed. See also code 5.
5 = UDP EXTERNAL: Step change if C-input signal becomes active and the beam is in
the upper dead point. Now you may move the beam and the retract function of theback gauge will be performed.
Delay time
Programmable delay time before step change (0-30sec)
Force
Maximum adjusted force during pressing (automatically computed).
Dwell time
Holding time of punch at bending point.
Decompression
Decompression stroke after bending to release the working pressure
Pressing speed
Working speed (pressing speed). Initially, the value for this parameter is copied from the parameter Default Pressing Speed in the Settings mode.
Decompression speed
The decompression speed is the programmable speed which is active during the programmed decompression stroke.
Part support return speed
Return speed of the part support after a bending. The speed value is programmed as a percentage of the maximum speed. Only available when there is a part support on the system.
Note
After selecting a new bend this will be a copy of the preceding one; you only have to alter those parameters which are different from the preceding bend.
Bend parameters – All Bends
When the function All Bends has been pressed, a complete overview of the bends appears.
After pushing End the page from which this page was selected will be restored, with the cursor on the parameter selected before.
Specific bend can be selected on the screen by putting the highlighted bar on that bend, then selecting END.
From within this screen, the complete CNC program can be edited. All bend parameters can be edited within the table and bends can be swapped, moved, added and deleted.
The available columns can be scrolled by finger movement / swipe.
Edit the program with one of the following commands:
• insert bend
• delete bend
• mark bend
Copy the value of the currently selected parameter in the current bend to all other bends.
Program the gauge positions, as already explained earlier in this chapter.
When the function Edit has been pressed a new, temporary button bar appears with additional functions:
To insert a new bend between one of the bends. When pressed, the current bend is copied and added after the current bend.
Mark the current bend, in order to prepare it for another action, like move or swap. See description below.
To delete the bend that is currently selected.
When a bend has been marked with the function key Mark Bend several other functions become available:
In the table overview of the bend sequence, it is possible to change the order of bends simply by moving a bend to another place. Select the bend that must be replaced. Then press the button Mark Bend and the bend is highlighted. Now select the right place in the sequence. When the correct bend is highlighted, press Move Bend. The bend will be inserted on the current place.
With this command, two bends can change place in the bend sequence. Move the cursor to one of the required bends and press the Mark Bend button. Then move the cursor to the bend
with which it must be swapped and press Swap Bends. If for any reason the action must be cancelled, press the function Abort Mark during the procedure.
Remove the mark from the currently marked bend.
A bend is no longer marked when the mark is aborted, when an action is finished or when this menu is left.
With the parameter Connect it is possible to create a 3-dimensional product. The control automatically executes the bend sequences in the different directions in succession. You program the control as follows:
1 Create the product in one direction.
2 Create the product in the other direction.
There are now two bend programs of one product in two directions. You connect these programs as follows:
1 Select the program with the bend sequence in the direction which you want to execute in the first place. You select the program of the product via the ’product library’.
2 Go to the ’edit program’ menu. Select the parameter ’connect’. Select the product ID of the product in the other direction.
3 Select the second program as in step 1. Repeat step 2. If you want to connect two programs, as in this example, you enter the product ID of the first program. The cycle is closed.
When you want to execute more than two programs in succession (not necessarily to create a 3-dimensional product) the second program must refer to the third. The third program to the fourth and so on. The final program of the cycle must always refer to the first program.
To produce products with connected programs the next four actions are necessary.
1 Select the first program
2 Select the Automatic mode
3 Program the amount of products you want to produce with the ’stock count’ parameter.
4 Push the Start key.
When the first program has been finished the second program starts automatically. The program counter indicates the remaining amount of repeats.
After changing program data the control will not automatically calculate:
1 Force
2 Decompression
3 Crowning device setting
4 Z-axis position offset
5 X-axis position correction
Parameters 1 through 4 are only automatically recalculated if the parameter Auto Computations Edit (see the Settings mode) has been enabled.
Parameter 5 is only automatically recalculated if the parameter Active Bend Allowance Table (see the Settings mode) has been activated. Corrections on the X-axis position can be edited with the parameter Corr.X (per bend) and G-corr.X (for all the bends of the active program) in the Automatic mode.
There is one exception:
When the parameter Bend Method is changed the Force and Decompression will be adjusted automatically.
In auto mode with the active program, production can be started. After entering Auto, the Start button can be pressed and production can begin.
The automatic mode executes the program automatically bend by bend after pushing the Start button. When selecting a different product in Products mode, which is in the library and has already been used for production, one can immediately switch to Auto and start production.
Every time after a different bending program is selected you must check your tools and tool positions in your machine. This is also indicated with a ‘check tools’ warning message when you enter the automatic mode.
In the header of the Auto mode screen the selected product is displayed along with the product description. At the top of the screen the bend selector shows the available bends in the program. By tapping the prefered bend the bend can be selected. The start button can be pressed to start from this bend. The details of the selected bend are shown in the available views.
The repetition of a bend and the connected programs, when applicable, are shown in the header of the screen. A connected program is also indicated in the bend selectors last position.
Following is a list of the available parameters in Auto mode.
Corrections
Corrections on angle values in this bending.
Angle corrections can be programmed for both sides of the machine, Y1 and Y2. When correction Angle 1 is entered for one side, this value is automatically copied to the correction Angle 2 for the other side. The correction for the other side can then be changed. When both angle corrections have been entered, the resulting corrections for Y-axis and parallelism are calculated. The corrections will be saved in the activebending program.
The angle correction should be entered as following examples indicate:
Programmed value of 90 degrees.
Measured value of 92 degrees.
-> Then it is required to program of correction of -2.
Programmed value of 90 degrees.
Measured value of 88 degrees.
-> Then it is required to program a correction of +2.
In case the angle correction database has been switched on, the control checks whether a correction exists for this type of bend in the database. The result of this check is prompted in the entry field:
• No stored correction.
No correction has been found for this bend
• Stored correction.
A correction that matches the current bend has been found
• Interpolated correction.
A correction has been calculated (interpolated) based on other existing corrections
If a correction is entered, it will be stored in the database. At each next bend with the same properties, this same correction will be offered.
The angle correction database can be found on the Program Settings page in the Settings mode.
Corrections on the Y-axis positions, in case absolute programming is used or bottoming is selected for a bend.
Corrections on auxiliary axis positions in this bending. In case bend allowance is activated (see the Settings mode) and a program has been entered in data preparation,
the X-axes correction values are the result of bend allowance calculation. The corrections will be saved in the active bending program.
The auxiliary axis correction should be entered as following examples indicate:
Programmed value of 200 millimetres.
Measured value of 202 millimetres.
-> Then it is required to program a correction of -2.
Programmed value of 200 millimetres.
Measured value of 198 millimetres.
-> Then it is required to program a correction of +2.
Correction on the crowning device.
Only available if a crowning device is present.
General correction of the angle, valid for each bend of the program. The value should be programmed in the same manner as for the correction per bend.
General correction on the Y-axis position, in case ’absolute programming’ is used and ’air bend’ is selected for a bend. This correction is valid for each bend of the program.
This is a general correction on the angle position of the part support. It is valid for all bends.
The correction is programmed here as an angle value, relative to the part support angle of the current bend. The correction is remembered as a percentage of the current angle.
If another bend is programmed or selected with a different angle, the correction value will be adjusted accordingly.
(Only available if a part support is present.)
General correction of the X-axis position, valid for each bend of the program. The value should be programmed in the same manner as for the correction per bend.
General correction on the crowning device.
Only available if a crowning device is present.
Select to use either Auto mode (disabled) or Step mode (enabled). In Step mode you have the same possibilities as in Auto mode. There is only one difference. After each bend cycle, the control will stop. To continue working, you must start the control again by pressing the Start button on the front panel of the control.
The stock counter is incremented or decremented after each end of a program cycle.
Selection of one of the repeated steps of one bend. Useful if a bend has a repetition value larger than 1. This parameter is visible when the function Select Rept. No. is pressed.
The auto mode screen is offering a diversity of views which, depending on ones production methode, can be chosen. When selecting auto mode for the first time, the main screen will appear. On the right side of the screen the available view modes can be selected. Following view modes are available:
The appropriate view can be switched from and to, not changing the bend data. The Start will not jump to Stop while switching view modes.
Main
Main view shows the numerical data of the bend along with the corrections. The corrections can be programmed here. The splitter control devides the screen in graphical visualisation and the numerical data. This can be closed if only numerical data is required.
Both lower columns can be scrolled to see all data. In the graphical view quadrant zoom, pan and rotate can be used to view the bend position in the machine.
The tool view quadrant zooms automatically in on the used tools. During the bending proces the tool station to be used will be indicated to help the user to select the correct station.
Bend selector
The bend selector in the top of the screen can be used to navigate thru the bends. The indicated bends can be tapped to easily select the desired bend data. In the bend selector the turn indicator will be displayed showing green, yellow or red colors to indicate the level of complying the assignments of the bend sequence.
All bends
The all bends view mode shows, with or without the opened graphical pane, a table including all bend data. The bends are shown row wize and the columns display all bend parameters.
During bending the control will step through the list and corrections belonging to the selected bend are shown in the lower part of the screen.
In graphical view mode a full screen graphical view of the bend process is given.
Optionally the view can be switched to 3D to have the product and machine shown in 3D. This can be toggled.
Changes to the view angle and zoom level will also be used in the smaller graphical visualisations in other view modes.
With macro view mode, the control switches to a view with only large axes values on the screen. This view can be used when working a little remote from the control, still able to read the axes values.
Next to the target position (programmed) also the actual position of all access can be followed.
In manual positioning view mode the axes values are shown at large. Axes can be selected and while selected the position can be controlled by turning the handwheel.
The teach indicator:
The manual positioning functionality can be expanded by using an external handterminal. This handterminal allows the operator to remotely control the handwheel functionality, including
axes selection and bend selection, and teach found axes positions to the program.
In this view mode all corrections of all bends are shown. You can browse through all corrections and change them as you see fit. If a correction for α1 is entered then this value is copied to the correction for α2. Different corrections for α2 can be entered in the field itself.
The column ‘Stored correction’ is only available when the Angle correction database has been activated. When activated, the column ‘Stored correction’ shows for each bend the correction value that is present in the database. A blank entry in this column means the database does not have a correction value for this type of bend. When a new correction is entered, it will be copied to the database automatically.
The markers ‘>’ indicate bends that have the same value.
All From Stored serves to copy corrections in the database to the current program: corrections in all bends are adjusted according to database values.
The function Bend Allowance helps the user to add entries to the bend allowance table in case this is active. Based on the active bend parameters only the bend allowance corrections needs to be entred before adding. With entering a measured value here, the resulting difference is translated to bend allowance, can be used.
To calculate the corrections from measured angle values, one can use the “calculate corrections” function in the correction window. Calculate corrections will open a separate window in which, upon choice, the measured angle(s) can be programmed.
From the programmed value the control will determine a correction. The proposed result can be seen in the window itself. In the top of the window the programmed angle is shown, in the
bottom of the window the resulting corrections are shown. When selecting accept, these values will be transferred to the main corrections screen.
When only one measured angle value is entered, the other values will be copied equally. If there are separate left, right or even middle values, these can be entered as well. The appropriate correction values will be determined from the entered values. The middle measured angle, if applicable, is transferred to an absolute crowning correction.
When using the optional protractor device, measured values can be taken directly into the correction field or can also been obtained within the “calculate corrections” window. After a satisfactory measurement, corrections are transferred to the main corrections window. If values are entered directly in the correction field, new corrections are only accumulated after a new bend cycle.
Tool setup shows the tool configuration which is required for the selected product. In the tool setup view mode also tool properties, next to their required position, can be checked.
In this tool setup view mode no changes can be made to the actual setup. If this is required one has to switch to the Tool Setup menu, outside Auto mode.
The diagnostics view mode is meant for service purpose mostly. In diagnostics the activities of independent axes can be monitored. I/O on the control system can be followed. In rare situations this information can be helpfull to diagnose operation during the bending proces.
In case of a selected bumping bend a general correction for a bumping bend can be entered. This function can be activated when the cursor is on the parameter for angle correction (‘corr.
α1/α2’). It is only available if a product is loaded that contains a bumping bend. With Bumping Corr. a new window appears in which the correction can be entered.
When the general correction of an angle is altered, all individual corrections are recalculated.When any of the individual corrections is altered, the general correction is recalculated.Bumping corrections can be programmed independently for both sides, α1 and α2. When the general correction α1 is changed, it is automatically copied to α2 and as a result, all separate corrections for α2 are recalculated. To change correction values of α2, use correction α2 or one of the separate corrections of α2.
In manual mode you program the parameters for one bending. This mode is useful for testing, for calibration and for single bends.
Manual mode is independent from Automatic mode and can be programmed independently of the programs in memory.
In the top of the Manual mode screen you can find the Y-axis and the main X-axis current position. All other axes and functions are listed one by one in the two columns below.
When these Y axis value or the X-axis value is highlighted it means that the reference markers of these axes have been found and that they are positioned correctly referred to their programmed values.
Manual Mode, Parameter Explanation
Following is a list of the available parameters in Manual mode.
Product Properties
Program the thickness of the sheet.
Selection of one of the programmed materials, which are used to calculate the bending depths. The control contains 4 pre-programmed materials. In total, 99 materials can be programmed on the control. The materials can be programmed on the Materials page in the Settings mode.
1) Method
Select the required bending method. The control supports 4 methods:
• Air bend
• Bottoming
• Hemming
• Hemming & bottoming
The bend methods have been explained in more detail on the Basic Data page in the Program mode.
2) Bending length
Program the bending length of the sheet.
3) Angle
Angle to bend.
4) Corr.α 1, Corr.α 2
Correction on angle to bend.
The angle correction should be entered as following examples indicate:
Programmed value of 90 degrees.
Measured value of 92 degrees.
-> Then it is required to program Corr.α with -2.
Programmed value of 90 degrees.
Measured value of 88 degrees.
-> Then it is required to program Corr.α with +2.
5) Corr.Y
Correction on the Y-axis position, in case bottoming has been selected.
6) Y-axis
The programmed or calculated Y-axis value to realise a certain angle.
7) Mute
Sequence point where the Y-axis is switched from fast closing speed to pressing speed.
It is programmed here as a Y-axis position value. The programmed value is the Y-axis point above the sheet.
8) Parallel
Difference of the left- and right hand side cylinder (Y1 and Y2). When positive, the right hand side is lower. When negative, the right hand side is higher. The programmed value is active below the clamping point.
Opening
This parameter results in a certain gap opening between the punch and the die after the bend. A positive value is the gap opening above Mute, a negative value below Mute.
When you want to limit the handling time for the product you can program a small positive or a negative value.
9) Hem opening
The hem bend can be made with a certain opening distance between the 2 flanges. The hem opening value will be used calculating the beam position in the hemming process. By default this parameter has the value of the Settings mode parameter Default Hem Opening.
Force
1) Force
The programmed force applied during pressing.
2) Dwell time
Hold time of punch at the bending point.
3) Decompression
Decompression distance after the bending to release the working pressure from the system.
Pressing speed, the speed of the Y-axis during bending.
The decompression speed is the programmable speed of the beam during the decompression stroke.
In case of a retract, let the Y-axis wait until the retract is finished, yes or no.
No: the retract is started when the Y-axis passes the clamping point, the Y-axis does not stop.
Yes: when the Y-axis reaches the clamping point, the Y-axis is stopped and the retract is started. When the retract is completed, the Y-axis moves on.
The name (ID) of the selected punch. Tap to modify or select from the punch library.
The name (ID) of the selected die. Tap to modify or select from the die library.
The name (ID) of the selected punch adapter. Tap to modify or select from the punch adapter library. Whether an adapter can be programmed depends on the parameter Use punch adapter in the Machine mode.
The name (ID) of the selected die adapter. Tap to modify or select from the die adapter library. Whether an adapter can be programmed depends on the parameter Use die adapter in the Machine mode.
The tool selection enables you to directly type the desired tool, or by tapping the list key on the keyboard, the library will be shown and a selection can be made. When typing, the filter function will narrow down your selection in order to rapidly find your tool.
Turn Punch can be used to turn around the applied tool (back to front). When this is done, and active, the indicator is shown behind the punch or die.
If you have one or more auxiliary axes (for instance an X-axis, R-axis, Z-axis or part support) the parameters of these axes appear here. When you have a R1-axis and a R2 axis the programmed R1 value is automatically copied to the R2-axis value. The R2-axis value can, if necessary, be changed afterwards.
The retract distance of the axis during the bend. The “backgauge retract” is started at the pinching point.
Speed of the axis in the current bend. Speed can be programmed in a percentage of the maximum possible speed.
This is a general correction on the angle position of the part support. It is valid for all bends.
The correction is programmed here as an angle value, relative to the part support angle of the current bend. The correction is remembered as a percentage of the current angle. If another bend is programmed or selected with a different angle, the correction value will be adjusted accordingly. (Only available if a part support is present).
Return speed of the part support after a bending. The speed value is programmed as a percentage of the maximum speed.
(Only available if a part support is present.)
The above mentioned parameters can be programmed and modified as required. After pushing the Start button the programmed parameters are active.
Parameters in manual mode can be programmed one by one. The effect of the parameter on other parameters can be computed either automatically or manually. This depends on the selected mode on the left-hand side of the screen. The Auto Computation switch enable to select between:
The relation between parameters is visualized with a symbol and a background color.
When an information symbol is shown with parameters after an editted value, this parameters was changed due to the last changed input.
A star symbol is shown with parameters if the value of the parameter differs from the calculated value by the control. This can be helpfull if a value is intentionally programmed different or if the value of a parameter is limited by the parameters limits.
A error symbol is shown with a parameters if the value cannot be correct according to the currently programmed values. This, eg. when a hemming bend is programmed with no hemming tools programmed.
The command buttons on the right side of the screen give access to other views. Next to the Main view, there are Macro, Manual Positioning, Corrections as also a Diagnostics view.
With Macro the control switches to a new view with only large axes values on the screen. This view can be used when working a little remote from the control, still able to read the axes values.
To move an axis to a specific position manually, the hand wheel on the front panel of the control can be used. After tapping Manual Pos in the main screen of Manual Mode, the following screen appears:
Within this mode, any of the shown axes can be moved by turning the hand wheel. The procedure for moving the axis depends on the axis you wish to move.
The control must be stopped (the LED on the Stop button is on).
First select the desired back gauge axis, you will see the cursor at the required axis.
Then you can move the axis by turning the wheel.
The pressbeam can be positioned manually in the same way as the auxiliary axes.
However, for the Y-axis several conditions must be met:
• The control must be started (the LED on the Start button is on).
• The ‘adjust’ function must be active, indicated on the screen by “Adjust” in the lower right-hand corner.
• The Y-axis must be below mute-point.
• A pressing command must be given to the CNC.
To teach the control, taking over a position found by manual moving an axis, a simple procedure can be used.
When you have moved an axis to a certain position with the hand wheel, you may want to store this position. To do so, tap the axis name in the Programmed column. The actual axis value (left side) will appear in the programmed axis field (right side).
When you return to the standard screen of manual mode, the axis parameter will have the recently taught value.
In this view mode the corrections for the bend programmed in Manual mode are shown. Since this is always a single bend, a single line will be shown.
The programmed corrections can be verified here similarly to the corrections in Automode.
Entries in the correction database and for initial correction can also be monitored in this screen. Since these are of significant influence on the bend result, access to the database can be used to modify. This can also be usefull while finding appropriate corrections with testbending and storing the found results in the database.
The function Bend Allowance helps the user to add entries to the bend allowance table in case this is active. Based on the active bend parameters only the bend allowance corrections needs to be entred before adding. With entering a measured value here, the resulting difference is translated to bend allowance, can be used.
When tapping Diagnostics, the control switches to a new view which shows axes states. In this window, the current state of available axes can be observed. This screen can also be active while the control is started. As such, it can be used to monitor the control behaviour during a bend cycle.
When tapping on one of the modules in the Diagnostics, the control switches to a new view with the state of inputs and outputs. In this window, the current state of inputs and outputs can be observed. This screen can also be active while the control is started. As such, it can be used to monitor the control behaviour during a bend cycle.
When tapping on one or more (up to 8) pins and extra page Zoomed IO is created with an enlarged view of the selected IO; selected pins will be shown in large, enabling distant monitoring.
By tapping the navigation button Settings the control is switched to Settings mode.
The Settings mode of the control, which can be found in the navigation panel, gives access to all kind of settings which influence the programming of new products and programs.
Default values and specific constraints can be set.
The settings are divided across several tabs logically organizing the different subjects. In the following sections the available tabs and detailed settings are discussed.
Navigation through the tabs can be done by just tapping them and selecting the required item to adjust. Since there can be more tabs than the screen can show in one view, dragging the tabs in horizontal direction enables to view and select all available tabs.
Select the required tab and tap the parameter to be changed. When parameters have a numerical or alphanumerical value, the keyboard will appear to enter the desired value. When the setting or parameter can be selected from a list, the list will appear and selection can be done by tapping. Longer lists allow scrolling vertically to check the available items.
Select to use either Millimeters or Inches as the unit to be used.
Select to use either Ton or kN as the main unit to be used for all force data.
Select to use the resistance either per meter or per millimeter.
The user interface language can be selected from the list. There are more available languages than initially shown. Scroll vertically by dragging the list up en down to see all available languages. Tap to select the desired language for the user interface. (For languages using special, non standard alphanumerical characters, the control will reboot.)
The help language for the on-line Help function is by default set to the same language as the user interface. If that language is not available as on-line Help, English is chosen. When Help Language is selected, the additional function Add Help Language appears.
With this function you can install a new help language on the control. Make sure the required help file is present on the control disk or another accessible location (network, USB stick). It will automatically be selected and installed.
Upon choice one can select Qwerty, Qwertz or Azerty keyboard layout. Default layout is Querty.
Switch the sound function of the input panel on or off. Default sound is on.
Switch the command panel to the left side of the screen. Default is right side.
In this tab, materials with their properties can be programmed. Existing materials can be edited, new materials can be added or existing materials deleted. A maximum of 99 materials
can be programmed on the control.
For each material, three properties are present and can be viewed and edited.
Name of the material, as it will appear in the programming screens. The maximum allowed length of the material name is 25 characters, the name must begin with a character (not a numeral).
Tensile strength of the selected material.
E- module of the selected material.
The materials are initially listed according to their material number, which is shown in the first column (ID). The list can be sorted according to the different properties by tapping the title of
the column. The materials will be sorted in ascending or descending order of that property.
To change an existing material, select the relevant line and change the values as you see fit.
To delete an existing material, select the relevant line and use Delete Material. This will erase the values.
To program a new material select an empty line and start programming its values.
This tab offers the possibilities to backup and restore products, tools as well as settings and tables. When products or tools originate from older control models, both for products and tools an import function can also be found here.
Tools and products can be backupped and restored according to the following procedures.
The procedures for saving or reading data are similar for all types of backup media: e.g. network or USB stick.
The actual backup directory consists of a device (USB stick, network) and a directory. The choice of devices depends on which devices are connected to the control. If necessary, directories can be created and selected. The backup locations for storage of products and tools are set independently.
To make a backup of programs to disk, choose Products from the main menu Backup.
When the initial backup directory has been set, the products backup screen appears.
In the backup screen the products in the selected directory are shown.Basic functions to change the view can be chosen similarly to the Products mode. This enables to easily find the required products to be backupped.
At the top of the screen, the current source location is shown as well as the backup location.
To backup a product, select it by tapping, in the list. The backup marker will appear to confirm the backup action. If a product file with the same name is present on the backup location, a question is offered whether or not to replace that file.
To backup all products at ones, tap All.
The source where the products are located which have to be backupped can be changed with Source Directory. The directory browser appears and the desired source directory can be navigated to.
The directory where the products which need to be backupped need to go can be changed as well. With Backup Directory the directory browser appears and the desired destination directory can be navigated to.
To restore programs to the control, choose Products in the main menu Restore.
When the initial restore directory has been set, the products restore screen appears.
In the restore screen the products in the selected directory are shown.
Basic functions to change the view can be chosen similarly to the Products mode. This enables to easily find the required products to be restored.
At the top of the screen, the current restore source location is shown as well as the location on the control to restore to. To restore a product, select it by tapping, in the list. The restore marker will appear to confirm the restore action. If a product file with the same name is present on the control, a question is offered whether or not to replace that file.
The source location where the products to be restored are coming from can be changed with Restore Directory. The directory browser appears and the desired restore directory can be navigated to.
The directory where the products which need to be restored need to go can be changed as well. With Destination Directory the directory browser appears and the desired destination directory can be navigated to.
To make a backup of tools to disk, choose Backup in the main menu for Tools.
When the initial backup directory has been set, the tools backup screen appears.
With this menu a back-up of tools on the control can be made: punches, dies or machine shapes. The procedures for a tool back-up run similar to the procedures for a product back up.
The restore procedures for tools run similar to the procedures for product restore.
To backup user specific settings and tables the Backup/restore tab offers specific functionality. The procedure is again analogue to the backup and restore of products and tools. The special
function All, will automatically execute all steps sequentially for either Backup or Restore (Products + Tools + Tables + Settings).
When Backup Directory is used, a new window appears with a list of available backup directories.
In this window you can browse through the directory structure of your backup device. Tap the dot to look inside a subdirectory. To move one level up, tap the (PARENT) map. To select the
directory you are currently in, tap Select. To change from one device to another, tap the (PARENT) symbol a number of times until the highest level is reached. From there, select the proper device and choose the correct subdirectory.
If a network connection is available you must first select Network and subsequently one of the offered network volumes. After that it works similar to other devices.
You can make new subdirectories or delete existing ones tapping Make Subdir and Remove. Subdir. If there are subdirectories present, just tap it to move to the required directory and tap.
Select to select it.
Parameter to enable the database with angle corrections.
Angle corrections are entered in production mode (Auto mode). These corrections are stored in the product program.
The Angle correction database enables the possibility to store these corrections in a database. In this way corrections that have once been entered for certain bends remain available for future use in other products.
With this setting enabled, the control checks during production whether corrections for similar bends are present in the database. If corrections for certain bends are available, then they will be offered. On other occasions, corrections can be interpolated and offered.
The correction database is adjusted by entering new corrections during production.
When the database is enabled with this parameter, all new-entered corrections are stored in the database.
When searching for similar bends, the control searches for bends that have the same properties as the active bend. The following properties of a bend are compared:
• Material properties
• Thickness
• Die opening
• Die radius
• Punch radius
• Angle
The first five properties of a bend must be exactly the same as the active bend to start a comparison. If the angle is the same as the angle of the active bend, the correction is offered. If the angle of the active bend has a maximum difference of 10° with two adjacent bends, a correction is interpolated from these two bends. If the difference of the corrections of the two adjacent bends is more than 5°, there will be no correction offered.
To program relative small angle corrections the initial correction database is available.
This parameter is independent on the parameter “Angle correction database”.
The initial correction is only visible and programmable on the corrections page in automatic mode. On the main page in automatic mode the initial correction is not visualized. The total correction is the sum of the visualized correction and the initial correction.
Example:
– Program an angle correction of -8 degrees.
– Program an initial correction of -6 degrees. Now the total correction
remains unchanged: the visualized correction is changed from -8 degrees to -2 degrees.
disabled => no initial angle corrections programmable.
enabled => initial angle corrections programmable in all corrections overview
To program general angle corrections which are used in all bends of the program.
These angle corrections are not related to specific bend angles and therefore not stored in the angle correction database.
disabled => no general angle corrections.
enabled => only G-corr. α1 (default).
α1 and α2 => G-corr. α1 and G-corr. α2.
To enable the storage of angle corrections programmed in Manual mode. Corrections can be derived from bend results in Manual mode which later can be used during product programming.
Parameter to switch between copying or keeping the delta values or changing independently when changing angle corrections in production mode.
copy => copy Cα1 to Cα2 when changing Cα1 (default).
delta => keep delta between Cα1 and Cα2 when changing Cα1.
independent => change Cα1 and Cα2 independently.
Parameter to switch between copying or keeping the delta values or changing independently when changing the X-axis corrections in production mode..
copy => copy CX1 to CX2 when changing CX1 (default).
delta => keep delta between CX1 and CX2 when changing CX1.
independent => change CX1 and CX2 independently.
In the Program mode you can change the value of the programmed parameters. This can also influence the value of other parameters. With this parameter set on you can choose to have the other values automatically recomputed.
There are three cases in which automatic computation can be used:
1. In case you change the value of the parameters ‘material type’ or ‘material thickness’ then the following parameters are automatically recomputed and changed by the control:
• Force
• Decompression distance
• Crowning device setting
2. In case you change the value of the parameter ‘length’ then the following parameters are automatically recomputed and changed by the control:
• Force
• Decompression distance
• Crowning device setting
• Z-axis position
3. In case you change the parameter ‘punch’ or ‘die’ and the height of the new punch or new die is different AND ONLY in case the ‘bend method’ is ‘bottoming’ or ‘hemming’ then the following parameter is automatically recomputed and changed by the control:
• Y-axis position (‘bend position’)
(When the ‘bend method’ is ‘air bend’ (normal situation) the Y-axis position is calculated in the automatic mode!)
If the Automatic computations edit is switched off (default situation) then these parameters stay the same. However, when you enter these parameters by tapping them the recomputed value is displayed. When you press ‘enter’ the recomputed value replaces the old value after all. So, you can choose to change the values.
Parameter to select in between angle programming or offset programming for the Xaxes backgauge. Only available when this option is installed.
angular format =>X-axes angle can be programmed projection method=>X-axes offset will result in an calculated angle.
When you have two independent X-axes (X1 and X2) and the option OP-W-X@ has been installed, you can program the values for X1, X2 in an angular relation. This means that you program X1 and an angle value (angular method) or in a projection measure.
Please ask the option description from your supplier when this option has been installed.
Parameter to program the two Y-axes independently.
off => single Y-axis programming (default)
on => program Y1 and Y2 separately
Default Y-axis opening value. The value programmed here is used as initial value for the parameter ‘Y-axis opening’ in the Program mode.
Default pressing speed, used as initial value for the parameter ‘pressing speed’ in a new program.
Default value for the parameter ‘wait for retract’ in a bend program. This parameter determines the control behaviour in a bend program. Initially the parameter ‘wait for retract’ is set to the value programmed here during postprocessing and during programming. The default value of this parameter: yes.
Default value for the parameter ‘step change code’ in a bend program. This parameter determines the moment of step change in a bend program. Initially the code parameter is set to the value programmed here during postprocessing and during programming.
The default value of this parameter is: UDP.
The step change codes have been explained in more detail on the Optional Data page in the Program mode.
During the postprocessing, the waiting time of the X-axis at step change is set to zero.
With this parameter you can preset a longer waiting time when needed for product handling.
Default value for the parameter ‘dwell time’ in a bend program.
Default value for the parameter ‘prebend angle’ in a graphical product.
The hem bend can be made with a certain opening distance between the 2 flanges. The hem opening value will be used calculating the beam position in the hemming process.
This programmed default value will be used when programming the product with hem bend graphically in the Drawing mode or by programming a new program in the Program mode. The starting value is 0.0mm to get the two flanges of a hem bend completely upon each other without any space between the flanges.
The default value of the parameter = 0.00
A graphical product drawing can be made in outside or inside dimensions. This parameter defines the default value of the parameter “dimensions (D1)” when creating a graphical drawing.
computation => the control will calculate the bend alowance table => the bend allowance table will be used
Bend-allowance is the correction of the X-axis due to sheet shortening after bending.
With this parameter the method for bend-allowance calculation is chosen. ‘Computation’
means the standard formula of the control is used to calculate the bend-allowance.
‘Table’ means a bend-allowance table with correction values can be used. The choice ‘table’ is only available if a bend-allowance table is present on the control.
correction off => no bend-allowance added to numerical programming
correction on => bend-allowance correction added to numerical programming
With this parameter you can choose whether or not you wish to have programmed values corrected for bend-allowance. This setting only refers to corrections during product programming in the Program mode. If a numeric program has been entered with Corrections On, the axis corrections are calculated and stored in the program. These corrections can be viewed and edited in production mode (see ‘Auto mode’).
This choice has no effect on the post process function in the Drawing mode. When the control post processes to calculate a CNC program from a drawing with bend sequence, the control will always take bend-allowance into account.When a bend-allowance table is present and the cursor is on the parameter Active Bend Allowance Table then an extra function is available: Edit Table. With Edit Table the table can be modified to meet user requirements. The table appears in a new window, with its own controls.
Each line contains a table entry, with several parameters. In this screen, the following functions are available:
Tab to select the field you wish to change. Then type the new value and press ENTER.
It is not possible to create a table through this menu. Only when a table has been loaded into the control is it possible to edit its contents.
For more information about bend-allowance tables, we refer to the Delem manual of the bend allowance table.
It is also possible to load a existing bend allowance table.
Tab Load Table to navigate to the desired file location.
The force needed for an air bend multiplied by this factor in order to obtain the bottoming force.
The distance from the edge of the finger to the corner of the sheet.
When automatic Z-axes are installed, the position of the fingers is automatically calculated with respect to the end of the sheet.
Setting for the stock counter in production mode, to have the stock counter (product counter) count up or down.
When down counting is selected, the stock counter in production mode is decremented after each product cycle. When the counter has reached zero, the control is stopped. On the next start action, the stock counting value is reset to its original value.
When up counting is selected, the counter is incremented after each product cycle.
Down counting can be useful if a pre-planned quota must be produced. Up counting could be used to give a report on production progress.
This parameter can be used to have automatic step change in the bending process with the Step mode enabled.
disabled => No automatic step change (next bending parameters active) will take place. To perform the next bending you must select the new bending and press the start button.
enabled => The next bending parameters are loaded automatically but the axes will start positioning after the start button has been pressed.
An overall parallelism, valid for the complete Y-axis stroke, can be programmed with this parameter. The programmed value will be checked against the maximum allowed value during production. The parallelism which can be programmed for each bending (Y2) is only active below the clamping point. The parallelism below the clamping point is the sum of the two parameters (Y2 + Parallelism offset).
To enable the locking of the touchscreen while the controller is started.
Percentage of calculated force which actually controls the pressure valve.
The position of the beam at which the sheet is clamped, is calculated. In order to have a firm clamped sheet it is possible to offset the calculated pinch point with the value here programmed. A positive value will result in a deeper position, a negative value in a higher position of the beam.
Return speed of the part support after a bending. The speed value is programmed as a percentage of the maximum speed.
Only available when there is a part support on the system.
Extra angle for the part support unit. This angle value is added to the part support angle position at the end of decompression. So while the pressbeam moves up to its uppe dead point, the part support moves to this angle. When the beam has reached upper dead point, the part support will move back to zero.
Only available when there is a part support on the system.
Temporary safe value for the X-axis, to avoid collision as a result of movement along the Z-axis. With this parameter a standard safety zone for the X-axis is defined, which is valid for all programs. The value 0 disables this functionality. This parameter should not be confused with the parameter ’X-safety’ of each die.
This parameter is especially useful when several dies of different sizes are placed on the machine. In that situation, this intermediate X-value should be larger than the safety zone of the largest die that is installed.
When the back gauge has to move to a different Z-position, it is checked whether the current X-position is safe. We can distinguish the following situations:
• Old X-axis position as well as new position outside the zone: X- and Z-axis movements happen at the same time, no change.
• Old X-axis position outside, new position inside the zone: back gauge is positioned on
Z-axes first, the X-movement starts when the Z-axes are in position.
• Old X-axis position inside, new position outside the zone: back gauge starts along Xaxis, Z-movement is started when X-axis is outside the zone.
• Old X-axis position as well as new position inside the zone: back gauge moves to the intermediate X-axis position, then the Z-movement is started. When the Z-axes are in position the X-movement is started to move the back gauge to its new position.
Temporary position for the R-axis, to avoid collision as a result of movement of the Xaxis. The value 0 disables this functionality. When programmed not equal to zero this position will be active when the X-axis has to move inside the safety zone of the die.
The sequence will be as follows:
• The R-axis is moved to the intermediate position;
• then the X-axis is moved to its intended position;
• finally the R-axis is moved to its intended position.
The safety zone of the die is defined as follows:
SZ = X-safe + SD
Explanation:
SZ = safety zone
X-safe = safety zone of the die
SD = safety distance, defined by machine supplier
In some situations it is required to show the bend step notes automatically when automatic mode is started and when a new bend is selected. When this parameter has been programmed as “enabled” the notes are shown automatically in automatic mode.
The parameters on this page are used to calculate the production time for a product in the bend sequence computation process . This production time depends on the positioning speed of the axes and the product handling times. The positioning speed is depending on machine settings.
Manual handling, turning of a product takes production time. This time depends upon the length and width of your product.
For a relative small product (in Z-direction) a top-bottom turn can be done quickly.
But a relative small product which is long (in X-direction) needs some longer time to turn from front to back or in a combination turn.
The turn time can be set in a table in seconds. For this purpose there are 4 length intervals (3boundaries) each with a specific turn time depending on the type of turn. Like the turn times you also can set the length limit boundaries.
Boundary 1/2/3
Threshold values for product size. For values between these boundary values different product turn times can be programmed.
Display date and time on the title panel, time only or no time at all.
Display the time in 24 hours or 12 hours format.
Display the date in dd-mm-yyyy, mm-dd-yyyy or yyyy-mm-dd format.
To adjust the date and time. Adjusting the date and time will also adjust the date and time of the Windows operating system.
—End
Masters in industrial manufacturing with 25 years of experience and 10+ awards!
