IV2012: work point in DXF of sheet metal part

[Anonymous]

We have a custom-made sheet metal punch consisting of a 5x5 matrix of 1/8" holes. We export flat patterns from Inventor as DXFs.

We normally make DXFs by creating a view of the flat pattern on a blank IDW template (no border, no title block, nothing) and export that view as a DXF. This lets us orient the view at will, unlike right-clicking on the flat pattern in the browser and selecting Save Copy As.

When the sheet metal guy assigns tooling in his software, he needs to get each punch to "lock onto" the corresponding feature in the DXF. Normally this isn't a problem, but it has been with this gang punch. The center hole of the punch needs to lock onto the correct hole in the DXF, and it can't always seem to do it. I've sat alongside the guy as he does this, and in his software the centers of the circles show up as dots/points. But on this punch, there isn't necessarily a dot in the center of every circle, and it's possible that the center hole, which really needs the dot, won't have one.

I've come up with a workaround for this: a work point in the IPT. In the attached part, it's feature Tooling1. The sheet metal guy confirms that if I include the work point in the DXF as a point (in the AutoCAD sense), he can lock onto it. However, I find that if I generate a DXF from the flat-pattern IDW, the point is lost. If I generate an ACAD DWG from the IDW and save the DWG as a DXF, the point comes through in the DXF. But that's an extra step.

Is there a way to export directly from IDW to DXF and not lose the work point? Or is this as good as it gets?

For the sake of simplicity, the attached part has no bends. I realize that if I did, I'd have to re-create the points in the flat pattern, but that's another discussion.

Thanks.

[jletcher]

Two things

1. u should save copy as in the flat pattern. You can arrange the flat pattern by using edit flat pattern definition.

2. when making the gang punch as long as you have one center as you should in the save copy options make sure IV_TOOL_CENTER is on.

This should give you what he needs plus you don't have to make an IDW.

[Curtis_Waguespack]

Hi andrew_buc,

To compliment all that jletcher has said, see this link:

http://inventortrenches.blogspot.com/2011/05/edit-flat-pattern-orientation.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

I gave the suggestion a try, and it does seem to work. I should mention that we try to orient flat patterns on dwgs so that if you bend the part as per the flat pattern, you end up looking at a face of the part that looks like one of the formed views, as in the attached files. We figure the sheet metal folks don't have to go through so many mental gymnastics that way. We've accomplished this in the past with flat pattern orientation (default, pivot left, backside, etc.) on the .idw, and it's involved some trial and error. By the same token, we orient the .dxf to match the orientation on the .idw. Am I right in thinking that that if I follow the suggested procedure, the exported .dxf will be oriented the same as the view on the .idw?

Is IV_TOOL_CENTER a registry key, a setting in Inventor, or what? In any case, I was able to get the tool centers to show up using the procedure in Curtis Waguespack's blog. Inventor generated tool centers for all 25 circles in the gang punch, not just the middle one, but the sheet metal guy says that's acceptable.

Is there a way to get a .dxf without the tangent lines? If not, the downside of removing the tangent lines in ACAD may still be less than the downside of the way we've been doing it. I assume that these settings can be saved in an .ini file?

Thanks!

[jletcher · Accepted solution]

ok a few pointers that some may not know..

When unfolding a sheetmetal part and it has a finish like #3 s/s we drafter know that the #3 finish needs to be up in the flat pattern.

To do this without guessing all you have to to is pick a face you want up then unfold. The face you select will be the up face of the flat pattern. as for the bend tangents and bend lines you need to set up a dxf option and save the configuration so it does it the same way all the time... this is what I have mine set at. You can turn on and off things here including the tool centers without the other step...

[Anonymous]

Hmm, I exported the DXF with options as per your suggestions, and the DXF didn't have the tool centers.

Attaching the current version of the part, the DXF, and a screen grab of the suggested settings as I currently have them on my system.

[jletcher]

Thats a pattern not a punch feature. you called it a punch feature. You said the punch you have is a gang punch thats what you need is a feature with that config. do you have a cut sheet on this punch? make a feature that looks just like it then insert that into your part then the gang of holes will have one center point for the punch press program to read.

[jletcher · Accepted solution]

Now if this is the way you want to do it turn this one on

[Anonymous]

I was having some semantic confusion over punch in the literal sense vs. punch feature in the Inventor sense. I'll need to go back to the drawing board and decide which approach I want to take.