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Sheetmetal Cut


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I was wondering, should I use a single sheetmetal cut feature that would have multiple holes and retangles on a single face? Is this proper modeling in Pro/E? It seems to work fine without any problems and, to me, it's much easier to define and have understood on down the road.

Steve C
If they are interrelated, I say go for it... I do this when I have clearance holes for things that must protrude mounted behind the face of the sheetmetal.

It makes sense to me, to tie them all into one feature, because if one changes, they typically all change, so you only have one (sometimes messy) redefine to hammer on.

Obvoiusly you need to use some judgement here... If you have more than a dozen entities, or the cuts are _very_ complex, do yourself a favor, and divide them into different features. It will make for much less hassle when the inevitable changes come...

Also, as a veteran of the sheetmetal wars, do yourself a favor (if you haven't already) and start making UDF's (especially for bend reliefs, and corner reliefs, slots, tabs, etc...), and saving sketches of your most irritating cuts... These can be big time savers in the long run...
If I put several holes and other cuts into one massive cut, will it slow down regen rates? Using those same holes and cuts, will this facilitate any ordinate dimensioning?

Steve C
Yeah I'd go along with putting multiple cuts into the same sketch if they are related. Like the cutout for a bulkhead connector and it's mounting holes. As far as regen I believe it's faster to put multiple cuts in a smaller number of sketches than to have a sketch for each cut or individual hole features. However, Sketcher performance drops off dramatically if the section becomes too complex; at least if intent manager is turned on.

I've tried the UDF route and haven't been very successful with it yet. You have to be very crafty in how the dimensioning and constraints are done to make the UDF reuseable in a variety of orientations and reference schemes. I should probalby invest more time in learning how to accomplish this. By contrast, saving sketches is easy and you can simply type in the rotation angle after you see what the default is.

Bernie, that's how I would have done it with Unigraphics, but someone once told me that Pro/E doesn't behave when you do multiple closed section cuts all at the same time. I pretty much have a three sided U shaped piece of sheetmetal and I have three cut features, one for each wall, with numerous holes/square cutouts on each.

Steve C
Bernie hit it right on the head...

Connector cutouts _should_ go with their mounting holes, anti-rotating features _should_ go with their through holes, etc...

As long as all of the cuts have the same depth condition, multiple closed loops will be fine. Don't try to do half a dozen thru next cuts and add your thru all corner reliefs at the same time though, or you are asking for trouble. I've seen it done, and regen, and work fine, but it is a _bad_ thing.

Rule of thumb: If the cuts are interrelated, go ahead and sketch them together, as long as you aren't talking about something horrendously complicated.

As far as facilitating ordinate dimensioning... I rarely use the driven dimensions anyway in sheetmetal, so can't help you there. Just pick your two baselines, and start grinding out your dims...

By the description of your part, it sounds like you got it nailed...

The UDF's I use are mostly for slots and tabs, and bend reliefs... We use mutiple vendors, and some like round pockets, some like square pockets, etc...

I've built a few UDF's that combine with mapkeys to sketch a wall, rip relieve both ends and add bend reliefs... YMMV... It's a little backward, but it works...

Sorry it's been a long time for this reply. Thanks to the both of you Dave and Bernie. I'd like to keep this discussion open because this module is where I spend most of my time during the day. I have made some great advances in the sheet metal pro/E world in the past few weeks and have come to believe that this package is head and shoulders better than any I've seen, so far. Somehow I'd like to get into the PTC sheet metal group of users for enhancements to this module. There is still many things to learn about 'how to' and 'when to' use some the many tools before me. I'd like to see some of yours and others design ideas when doing inset flanges (flanges set into flat face not on edges).

Steve C
I too, spend, much of my day in the sheetmetal module...

Good for you that you've gotten comfortable using it. I too, believe it to be one of the best...

I'm not sure I know what you mean by an inset flange.

If you are talking about a recessed area for a flush access plate or something. I usually create the cut for the mating piece of sheetmetal, sweep the flange, and then rip or cut the corners out.

If you have a diagram, or could sketch something up real quickly, I'm sure we could set you off in the right direction...

I'm having trouble outputting a jpeg to show you. The best way to describe an inset flange is to take a flat piece of metal and cut a rectangle in the center and then add a flange inside the rectangle bent up or down.

Steve C
OK, gotcha. I'm assuming that you aren't looking for pieces welded in to square off your corners... Give me a few hours...

For an inset flange I think the best think to do is sketch your relief first. Then use the resulting edge to add a flange like normal. If it's a ripped and formed flange like you'd get from an N/C form tool you'd just cut a rectangle the width of the flange and the height less the setback (x-factor, shrinkage, whatever you calling).

That's what I've done, Bernie. Sketch the relief and then add the flange. I just wanted to see if there were any other ways. Obviously, when I get a little better at Pro/E, I'll make a UDF of a cut and just make adjustments there after.

Steve C
Well thanks Dave. I sure like making things easier for myself, but I need to get some basics under my belt before I go off the deep end with UDF's.

Steve C
No Steve...

I was going to send a model using Bernie's method outlined above... Not send a UDF...

I'm not sure if my UDF's would make any sense to anyone but me, anyway... (much like my extra-special-super-custom-yippee-ki-yay mapkeys...)

Let me know if you have trouble.

OK, I undertsnd now. It was beer-thirty when I answered your reply. I'm not having any troubles, just wanted to see if anybody else had a different method.

Steve C
If someone has some spiffy UDFs that would make a good reference for a sheetmetal library it'd be great if you'd post them here. I've beat my head against the wall a couple of times trying to get over that hump and just fallen back on the save a sketch routine. It just seems really hard to constrain the feature in such a way that it's easy to reuse in different orientations, different references, etc.

I've got a half-dozen or so, that I use all of the time... Like I said before, though, I'm not sure how helpful they'd be to anyone else.

They are relatively poorly documented (prompsthat say Pick the start surface stoopid..), and things like that. If there is interest though, I could try to clean up the ones that aren't hooked into my mapkeys and publish them.

I, as well, think that a good library of saved sketches (especially for d-subs, mil-spec connectors, reliefs, etc.), is far more valuable than the UDF's, but if there is interest, let me know...

I would be interested in seeing them, if for nothing else, to help me better understand how they are created.

Steve C


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