Troubleshooting Flat Pattern Sheet Metal Fold Tool breaking holes punches

[Hunteil]

In Sheet Metal, I have a folded piece of metal angled for a helical curve (spiral) with holes cut / punched throughout it.

• I used the fold tool at the diameter I needed.
• Then I generated a Flat Pattern for my .idw and then inside the flat pattern I right clicked, "Edit Flat Pattern Definition" and choose the alignment side so it's not randomly rotated.
• I open my idw, dimension everything on my flat pattern. The hole table it a bit finicky, and found that punches, you have to include "Punch Center" / center points / "Center Marks" when inserting the view. Then as a workaround, I have to physically add Center Marks to each hole. Then create the hole table. (again including center mark options)
• Final Result:

So here's the issue.

If I return to the .ipt and roll back my cuts and edit some holes or add cuts, I receive the error

I accept the error b/c I know I'll roll it back to end and everything will be fine. But when I do. Everything on the flat pattern becomes messed up and all the punch centers will not return and I can't get them to come back on the idw.

My troubleshooting attempts were:

• idw: I turned off and on the view setting for Punch Centers and still broken.
• idw: Manually re-adding center marks directly and it wouldn't do it. (But the round holes would let me.)
• idw: Deleting the flat pattern view and creating a new view and still broken.
• idw: I created new hole tables and still broken.
• idw: I created a new idw and place the flat pattern with Punch Centers and still broken. (which means it's the ipt from this evidence)
• ipt: Deleted the flat pattern and generating a new one and still broken.

For my project, I needed to build this quick, so I gave up and made a new .ipt and made all the changes up front without folding and no flat pattern until the very last step and it worked just fine!... But now I'm terrified that this will happen again if I need to edit it....

AND IT DID!

There is clearly something wrong... can anyone else confirm this is a bug / glitch? or am I doing something wrong?

Almost solution?: I tried right clicking the flat pattern in the ipt and picked "defer update". This looks to break the link so you can modify without that error. I did this and made my changes once and it worked! The next however it still broke...

[blandb]

Can you post your files?

[Hunteil]

Okay I got it cleaned up some for this. Here's the .ipt. You can just drop this flat pattern into any idw and turn on the punch center marks as you place it. You should see cross hairs (center marks).

[johnsonshiue]

Hi! I see the issue now. The problem is that the Fold feature makes the whole part bent. The only stable solution I can think of is to add those holes and cutouts in Flat Pattern only, not in the folded body.

Essentially, you will need to create two parts. One is folded with cutouts and the other one is the flat pattern with cutouts.

Many thanks!

[IgorMir]

Hi Noah;

There are two questions I would like to ask regarding your file:

1. I couldn't work out - why the Origin Geometry of the file is on an angle. That's something I don't recall seen.

2. Did you try to create a part in a folded shape from the beginning? Than use Unfold tool, do all the cut-outs on the part and after you are done - Refold it back. But be aware - the Unfold/Refold tool changes position of the part in space. You have to pick up a stationary reference very carefully when using this technique.

Cheers,

Igor. 

[Hunteil]

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@IgorMir wrote:

Hi Noah;

There are two questions I would like to ask regarding your file:

1. I couldn't work out - why the Origin Geometry of the file is on an angle. That's something I don't recall seen.

2. Did you try to create a part in a folded shape from the beginning? Than use Unfold tool, do all the cut-outs on the part and after you are done - Refold it back. But be aware - the Unfold/Refold tool changes position of the part in space. You have to pick up a stationary reference very carefully when using this technique.

Cheers,

Igor. 

---

In reference to your #1, are you talking about the origin geometry on an angle being in the flat pattern?, Oh I see what you mean. So after I made the geometry and folded it. I used "Look at" command on the face of the edge. Then right clicked the 3D navigation cube and set view as front... this changed all my USC, but kept my original sketch USC correct to the plate itself. I don't believe this caused any issues... But if you guys find it does, let me know... I only did this so my front and top view details looked correctly in the .idw. Otherwise it would look skewed and make it hard to dimension from the top view.

In reference to your @#2: So we tried the Helical curve in 3D sketch first, but found it nearly impossible to apply the holes using 3D sketches and not having the option to use "Arc Curve" constraints. We ended up unfolding that part but I think we couldn't get it to project surface lines or something. So we gave up on that technique (due to time). Someone else recommended only use sketches, cut everything there, then bend it with the fold tool after everything is done. Which as you can see works. But the flat pattern/hole table is throwing that problem as you can see.

[Hunteil]

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@johnsonshiue wrote:

Hi! I see the issue now. The problem is that the Fold feature makes the whole part bent. The only stable solution I can think of is to add those holes and cutouts in Flat Pattern only, not in the folded body.

Essentially, you will need to create two parts. One is folded with cutouts and the other one is the flat pattern with cutouts.

Many thanks!

---

So @johnsonshiue, this sounds like a cumbersome workaround which defeats my 3D assembly purposes... I need these holes/cuts shown for our 3D assemblies to our customers and for us to design direct parts for...

[Hunteil]

I ended up with the glitch again. The image is how I dealt with the issue... But it was extremely cumbersome to create b/c I had to create sketches with dumby circles for the center marks to stick to... (using projected with lines didn't work at all) And now as you can see, the view is very crowded b/c I have to use center marks in the flat pattern to get the table to recognize them and it insert leaders to each of them inside of the simple letters. 😞

I wish Autodesk would make the hole tables more functional in general.

On a 2nd note to using this fold technique. This is making my assembly literally impossible to constrain... I can use the center line of the arc, but none of the holes let me constrain to them...

[blandb]

Good evening,

If this has already been pointed out I apologize. But what if you tried the workflow below:

First just sweep a coil of a line the height of your side rail:

Next, just use the Thicken command and set the direction of either inside/outside of the surface typing in "Thickness" for the offset value so it is associated to your sheet metal defaults:

Now, use the unfold command and choose a stationary reference, add holes and rectangular pattern the holes:

Right-click on your unfold and choose refold and you now have holes and centerline axis along with origin planes to use for constraining:

Finally, place the flat pattern into the drawing and use hole table:

Hope that helps!

[andrewiv]

To your constraint problem, if you create a surface extrusion of a cylinder through your holes then you have something to use for constraints.  If you use joints I think you could actually select the middle and both ends of the holes.

[IgorMir]

Hi Noah;

Thanks for the clarifications.

For the UCS looking skewed - it just  looks odd on a screen but shouldn't create much of a problem. Unless you derive the part in your follow up design.

As for the creating the item as a spiral first - there is no need for 3D spiral at all. I would have sent you a sample file but it is in IV 2020 format. Yet Brad Bland has posted some screen shots of his part. My one looks pretty much the same.

Cheers,

Igor.