When it comes to optimizing your metal bending processes, understanding how to effectively manage the bend sequence with a DELEM DA-69S controller can make a significant difference. If you’re searching for ways to improve the efficiency and precision of your press brake operations, you’ve come to the right place.

In this article, I’ll guide you through the key aspects of optimizing the bend sequence using the DELEM DA-69S, ensuring that your workflow is not only streamlined but also achieves the highest quality results. Whether you’re a seasoned operator or new to the field, this guide will equip you with the knowledge to maximize your machine’s capabilities and enhance your metalworking efficiency.

Introduction

When a tool configuration is set, the bend simulation can begin to determine a bend sequence for the active product by tapping the ‘Bend Sequence’ navigation button. This can be done either by automatic calculation from the final bent product or manually starting from the flat product.

In the screen, you choose from manual programming, automatic computation, automatic computation with tool optimization, or with renewing the tool setup. The computation unfolds the product from the last bend to the first, either automatically or with function keys. If programming manually, it starts with the unfolded product.

Main Bend Sequence Selection Options and Functions

The DELEM DA-69S is equipped with several functionalities that facilitate the selection and optimization of bend sequences. Understanding these options is key to utilizing the full potential of the system.

Manual: The bend sequence must be programmed manually by the operator.

Sequence Only: Calculates a bend sequence based on the existing tool setup.

Sequence + Tool Optimization: Utilizes existing tools to optimize tool positions and tool stations for an optimized bend sequence.

Sequence + Tool Setup: Removes existing tools and calculates an optimized bend sequence using the best-fit tools from the library for each bend.

Computation Control:

• Cancel: Available when no valid bend sequence has been computed.

• Stop: Shown when a valid, but not time-optimal, sequence has been computed.

Functions:

• Unbend: Unfolds the current or next feasible bend.
• Bend: Simulates bending or progresses to the next step.
• Assignments: Accesses parameters for computing the bend sequence.

• Bend Sequence Functions:
  • Resume Computation: Computes a valid sequence starting from the selected bend.
  • New: Starts a new sequence, removing any existing one.
  • Reload: Restores a sequence from disk, ignoring related CNC programs.

After a bend sequence has been calculated or determined, the Save and Save as can also be found in this menu.

• Save: Saves the full sequence and its CNC program details once complete.
• Save As: Saves the product and sequence under a new name for easy differentiation.

Show bend sequence: 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

The view select option in the DELEM DA-69S allows operators to visualize the product and bending process from various perspectives. Within the screen views can be switched upon required choice. The view functions are located opposite of the command buttons in the main screen.

View functions:

Bend Selector

In the screen, bends can be selected and navigated using the bend selector. The top of the screen displays the number of bends with preliminary selectors. Once the bend sequence is complete, these selectors become active, colored, and show a turn indicator.

Bends can then be tapped to access desired data. The turn indicator in the bend selector uses green, yellow, or red colors to indicate compliance with the bend sequence assignments.

Unbend Product

The ‘Unbend Product’ function is a unique capability of the DELEM DA-69S that allows operators to reverse-engineer bending operations. By simulating the unbending process, operators can visualize the flat pattern and adjust bend sequences to optimize for manufacturability and material utilization.

To generate a CNC program, the bend sequence must first be determined. There are two ways to do this:

1. Automatic Computation: Press the function key ‘Compute’ to automatically find the quickest bend sequence.
2. Manual Unbending: Press ‘Unbend’ repeatedly until the product is completely unbent. Then press ‘Bend sequence’ followed by ‘Save’ to generate and save the CNC program.

If a bend sequence cannot be found, consider these potential issues:

• Incorrect tools: Update the tool configuration in the tool menu.
• Incorrect assignments: Modify assignments in the assignments menu.
• Collision during unbending: Manually adjust the bend sequence with available functions.

Manual Selection of Bends

The control system typically suggests the next (un)bend in a sequence, based on the programmed assignments, product shape, and tools used. However, there are cases where selecting a different bend is necessary.

The bend sequence can be adjusted using the manual selection features in the bend simulation menu. You can either:

• Start from a bent product and specify the desired unbend sequence.
• Start with a flat sheet and specify the bend sequence by tapping the bend sequence button and selecting ‘new’ for unbending or ‘new flat’ for bending.

The ‘manual bend sequence mode’ is active by default in 2D view and must be enabled in 3D view. Other modes available in 3D view, like ‘shift gauge mode’ and ‘shift product mode’, disable the manual bend sequence.

From a bent product, tap any bend to add it to the unbend sequence, with the sequence starting from the highest bend number to bend 1. For a flat product, tap any bend to add it to the bend sequence starting from bend 1 to the highest bend number.

• Bends that can occur without collision are indicated with a green circle.
• Bends resulting in a collision have a red circle.
• Yellow circles indicate bends that may need adjustments to avoid collisions.

Tapping a bend that is already in the sequence will select it, allowing you to continue from there.

Functions:

The following functions, available for modification of the bend position, are shown in the screen when active.

Shift Product and Shift Gauge

The ‘Shift Product’ function lets operators adjust the positioning of the workpiece, which is especially useful when fine-tuning bend sequences for complex geometries.

Functions:

• Shift product: Move the product by dragging it to the desired position, upon choice under a different tool station.

• Undo: Undo the last change to the product position.

The ‘Shift Gauge’ option allows for the precise positioning of the backgauge system, essential for achieving high accuracy in bend sequences, particularly in multi-stage or complex bending operations.

The fingers can be moved by means of the different available functions.

Functions:

• Select finger: Select the finger to move.

• Shift finger: Move the selected finger by dragging it to the desired position.

• Change side: Alters through the available backgauge positions.
• Lay on finger: Alters through the available product lay on positions. This option is only selectable in case you have an R-axis in your machine.

• Pinch corner

• Undo: Undo the last change to the finger position.

Assignments

Assignments are parameters that control the bend sequence computation. Access the assignments screen from the bend sequence screen using the ‘Assignm’ key.

Automatic computation of the bend sequence aims to optimize production time and handling, while avoiding collisions between the product, machine, and tools. To achieve optimum results, you must configure several parameters related to machine settings, product accuracy, handling possibilities, and turn times.

Functions:

• Load Defaults: Retrieve default assignment settings optimized for your situation. Store a preferred set using ‘Save as Default.’ You can apply these settings to new products by selecting ‘Load Defaults.’

• Save as Default: Store the current settings as your default assignment values.

• Cancel: Exit the current screen without saving changes.

• Accept: Save changes and exit the screen.

Assignments – General

Optimization 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 optimization, fastest computation

2 – low optimization, fast computation

3 – medium optimization, medium computation

4 – high optimization, slow computation

5 – highest optimization, 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 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 you can optimize this computation.

Tool length tolerance

Tool length can be shorter than the bendline length, but there is a programmable tolerance for the maximum difference allowed. This tolerance affects the bend sequence; if a tool’s length is shorter than the permissible tolerance, it will be rejected for that bend. The difference between the punch length (PL) and the bending length (BL) represents the tolerance value.

Product-product collision

Specify if product-product collision must be detected:

• disabled: product-product collision detection is disabled.

• treat as warning: product-product collision detection is enabled, and a product-product collision is treated as a warning.

• treat as error: product-product collision detection is enabled, and a product-product collision is treated as an error.

Minimum Y Opening
Set a minimum opening for the press beam during post-processing. This value is above the speed change point (Mute).

Unfolded Dimensions Limit
Define limits for Y opening based on product boundaries. For large products exceeding these limits, the opening is based on side length to avoid tilting.

Sheet Thickness Limit
Set limits for Y opening based on product boundaries. For thick sheets beyond this limit, the opening is based on side length to prevent tilting.

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

• Permit if unavoidable: 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 applies to press brakes with backgauge fingers on a moving R-axis (“lay-on” construction). If the sheet length behind the machine exceeds this limit, the X-axis and R-axis positions are automatically adjusted so the sheet rests on the backgauge finger, provided an automatic R-axis is available.

Minimum Finger-Product Overlap
Ensure a minimum overlap between the backgauge finger and the product to prevent unnecessary parking during bend sequence calculations.

Retract Optimization
Enable retract optimization during post-processing to refine graphical bend steps. When retracting towards the next bend’s backgauge position, the new position is used as the retract point, preparing the backgauge for the subsequent bend. This feature is off by default.

Simultaneous Bends and Group Selection

In addition to automatically selecting simultaneous and constrained bends, the bend simulation menu offers a grouping function. By selecting the unfolded view, users can manually select, deselect, and group bend lines, even if they aren’t aligned for simultaneous bending. This is useful for customizing bend sequences. Automatically grouped bends can also be ungrouped to allow for separate bending of lines.

Show bend sequence

When the function Show Bend Sequence has been pressed, a graphical overview of the bend sequence is shown.

Graphical Overview Function
This feature can be accessed anytime after the first unbend. The graphical overview displays both determined and undetermined bends, marked with a question mark. Each image can be individually enlarged, reduced, or rotated using touch gestures.

Frequently Asked Questions(FAQ)

Conclusion

Optimizing your bend sequence with the DELEM DA-69S involves leveraging its graphical overview and bend grouping functions. These intuitive tools assist in managing complex bending tasks efficiently.

Proper setup and utilization of the DELEM DA-69S features can help minimize errors and enhance productivity. For further assistance or to enhance your bending operations, feel free to contact our support team or explore our detailed documentation.