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Bend Line Dimension in Flat pattern

Question asked by Pardeep Yadav on Dec 12, 2018
Latest reply on Dec 17, 2018 by Scott Leacox

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I am attaching an image of error happening with me quite frequently. I am also attaching DXF of this parts which shows extra lines. That makes sense because those floating dimensions are not dangling.

Bend line dimensions are not updating automatically. Sometimes they float and lose their reference.

my process is "pack and go" the existing part, change the dimensions using design table and print the drawing. Then drawing goes to the shop floor. Sometimes I send drawing without checking.

For now, I am giving these dimensions manually in all drawing but I do want to use my standard process to reduce designing time.

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Keith Stegemann Dec 13, 2018 9:39 AM
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Boy...I've tried to help you out here buddy by duplicating the same as shown in your *.png attachments. NG...can't do it! I generate dxf files all day long of flat patterns for programming on a turret punch machine or a laser cutting machine so I'm well versed on how to get what I need.

Additionally...you write, "Sometimes I send drawing without checking." I, personally, will send NOTHING without checking! I've been in manufacturing for 44 years and trust NO software. I've been doing it a lot longer and know how to verify the integrity of a flat pattern. In the seven plus years that I've been with my current company. Not one program has left my office that can't produce a part[s] in a cost effective manner.

Good luck...I'll be watching this thread.
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Deepak Gupta Dec 13, 2018 9:48 AM
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Can you attach one file (both part and drawing) showing the issue?

How can I attach a file to a forum post?
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- Pardeep Yadav @ Deepak Gupta on Dec 13, 2018 3:42 PM
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  Attached.
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Taylor Duran Dec 13, 2018 9:51 AM
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When you're saving your dxf files are you saving the flat pattern view as a dxf or are you using the Export to DXF function from the model?

If you're exporting from the model, when you don't want the extra lines you need to select which entities you want to export.
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- Pardeep Yadav @ Taylor Duran on Dec 13, 2018 3:44 PM
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  I usually create one drawing named DXF and put flat pattern there in 1:1 ration and then save it as a DXF file.
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  - Taylor Duran @ Pardeep Yadav on Dec 13, 2018 3:53 PM
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    Maybe I don't understand what the purpose of your dxf file is for, but if you're using the dxf to program on a laser/plasma/water jet/punch like what Kieth was saying, I think you'll find that exporting the dxf straight from the model to be more efficient. For cutting a flat pattern, you I don't think you'll need the bend lines & notes that would be on the drawing.
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    - Pardeep Yadav @ Taylor Duran on Dec 13, 2018 4:06 PM
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      it is sometimes necessary to decide good face and put some notes for providing slits for bending people. One more thing is that I can put DXF of all parts within the assembly in one DXF file.
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Deepak Gupta Dec 13, 2018 4:20 PM
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This looks like a bug similar to one reported under SPR 489644. Please report to your VAR to check it in more details.

Can you try using a simple feature instead of loft and see if that resolves the issue?
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- Pardeep Yadav @ Deepak Gupta on Dec 13, 2018 4:43 PM
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  Thanks, Deepak.
  
  This profile tapers sometimes, I mean it is not necessary that dimensions on LHS match with dimensions on RHS. that is why we are using the loft tool.
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  - Deepak Gupta @ Pardeep Yadav on Dec 16, 2018 9:51 AM
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    I can replicate the issue, so report to your VAR.
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Kevin Chandler Dec 17, 2018 7:59 AM
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Pardeep Yadav wrote:

I am attaching an image of error happening with me quite frequently. I am also attaching DXF of this parts which shows extra lines. That makes sense because those floating dimensions are not dangling.
Bend line dimensions are not updating automatically. Sometimes they float and lose their reference.

my process is "pack and go" the existing part, change the dimensions using design table and print the drawing. Then drawing goes to the shop floor. Sometimes I send drawing without checking.

For now, I am giving these dimensions manually in all drawing but I do want to use my standard process to reduce designing time.
Although we all get rushed from time to time, I'd suggest always doing a review before printing.

One suggestion for reducing drawing time would be to not dimension bend lines.
Bend lines are basically imaginary creatures and if they are to be dimensioned, these should be reference dimensions.
Even if bend lines were accurately reliable, only the first line in from a real edge would be usable. The chain dimensioning basline disappears with each bend.
The bed lines only remain in place at the neutral plane within the part's thickness.
Instead, dimension (and tolerance) the final part as its shape and function require.
This is the document that determines whether the part is in spec or not.
Let the fabrication people use their expertise to make these parts happen.

Kevin
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- Scott Leacox @ Kevin Chandler on Dec 17, 2018 9:28 AM
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  Bend line locations are critical in my shop. They use them to program folding machines.
  I am still doing production work in solid edge starting a transition to works. In edge I have a system in place to actually present the back gauge and stick out information on the drawing for every bend. Complex when parts have more than 8 bends.
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  - Deepak Gupta @ Scott Leacox on Dec 17, 2018 11:01 AM
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    S. Leacox wrote:
    
    In edge I have a system in place to actually present the back gauge and stick out information on the drawing for every bend.
    Can you share more details on how you do that and how does that help the shop floor people?
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    - Scott Leacox @ Deepak Gupta on Dec 17, 2018 12:39 PM
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      It helps the shop people because they have to manually program a folder for every part. I give them a dimension as to where the put the back stop. And I give a dimension they measure with tape that is how much the part is out of the machine (The stick out). The two dimensions add up to the length of the flat at the state of bending the part is in during that bend. Also as part of the drafting I present what direction each bend is and what the bending sequence is.
      
      I don't know if this can be done in Solid Works. Works is much more limited in how variables flow from model to draft. Getting variables to become "global variables" is the typical shut down point.
      
      Attached is a screen shot that shows the process. The math varies depending on the shape and bending sequence.....it takes some getting used to to set up.
      
      Here is the main trick: For the first bend, the back gauge and stick out are simply the distance from the edge to the bend line. For subsequent bends along the same line, the back gauge or stick out is dimensioned to the tangent line with a radius and thickness added to it.
      
      Note that the bending dimensions are very dependent on the Thickness, Bend radius, and K factor. The location of the tangent lines where the bends start and stop have a direct influence on the numbers. If the part changes it does automatically update. But if the bending sequence changes, the math has to all be set up again.
      
      Also worth note, the labels on the sheet metal views are automated text extracting information from the part. In Works it's impossible to display the Gauge of the part in draft much less combine that with other information then display it. The imbedded information was also used to create cut lists/BOM's (same thing in my existing drawings)
      
      Big picture: All of the part names are generic so that I can copy the design, rename the drawing, re-size and re-gauge the design, then just update the print mostly automated.
      
      My entire system is being abandon going to a new system of drafting and modeling in Works. In works, every part must get it's own part number and be drafted on it's own. We are also abandoning the bend tables for the switch in platforms. I can't wait to see how that goes.
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      bending-edge.png202.1 KB
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Bend Line Dimension in Flat pattern

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