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Problem in Extrude command in Creo 2.0

anshulpro
1-Newbie

Problem in Extrude command in Creo 2.0

proe.jpg

Problem1-> Why cant creo extrude the closed loop in any of the three surface...i dont find any pblem why its should not extrude in the above part.

save_pic.png

Problem2-> Now, if i sketch in the other plane and extrude towards the solid creo shows an weird logic for solid modelling....i mean if the distance is less than 20 solid extrudes...if its greater than 20 solid extrudes.....but why it fails if extrude distance is same as the width i.e 20....:((((((

CAN ANYONE EXPLAIN WHY CREO IS BEHAVING IN SUCH A WAY ?

1 ACCEPTED SOLUTION

Accepted Solutions

I was able to duplicate this fairly easily with 2 simple extrudes. And yes, this has always been an issue when you have a coincident edge like that. In short, it represents 2 solids and it doesn't want to join them.

But it is more than that.

I put a revolve feature along that edge and it has a similar problem. Only when the feature was the full length of the "seam" -and- rotated at least 180 degrees (90 should have done it but didn't), then the 2 bodies would re-join. Once it is a single solid body, you can make the feature you wanted in one of many ways.

So short story, avoid this kind of separated geometry. The taper on the sides of the vertical body makes my revolve fix a little less attractive but with a little extra work it can all be done. But for simplicity's sake, start the horizontal body over.

You have simply run across a situation that Pro/E, WF, and Creo simply doesn't want to handle. Awareness of this, and other tangency limitations will get you a long way to making successful and sustainable designs.

re-join.PNG

View solution in original post

6 REPLIES 6

Please attache your model to the post. I'm sure we'll find someone on the forum that wants to take on the challenge

I was able to duplicate this fairly easily with 2 simple extrudes. And yes, this has always been an issue when you have a coincident edge like that. In short, it represents 2 solids and it doesn't want to join them.

But it is more than that.

I put a revolve feature along that edge and it has a similar problem. Only when the feature was the full length of the "seam" -and- rotated at least 180 degrees (90 should have done it but didn't), then the 2 bodies would re-join. Once it is a single solid body, you can make the feature you wanted in one of many ways.

So short story, avoid this kind of separated geometry. The taper on the sides of the vertical body makes my revolve fix a little less attractive but with a little extra work it can all be done. But for simplicity's sake, start the horizontal body over.

You have simply run across a situation that Pro/E, WF, and Creo simply doesn't want to handle. Awareness of this, and other tangency limitations will get you a long way to making successful and sustainable designs.

re-join.PNG

Bari
12-Amethyst
(To:anshulpro)

If you go to Geometry Checks you'll find a warning about non manifold geometry in that edge.

qw.jpg

I guess I'm missing something. This is what I created to duplicate but would still like to see the model. I received no errors or warnings when I completed the feature.

8-26-2012 11-53-11 AM.png

Adam, you are creating a cut where Anshul was filling in the void. Indeed, I was able to cut that section out of an "L"-shaped solid and it acted like a single solid object until you again try to fill it back in.

Back in 2000i you could not separate bodies which was really sad as I often separated solids into multiple segments with wire EDM. I am very happy that this separation capability was added. A little more care in programming regarding joining bodies would also be nice. I was actually surprised the revolve worked and it may be a fluke. I for one see this as a borderline bug and wouldn't mind seeing it reported.

Just to take it a step further, I made a radial pattern of 36 individual blocks, each separated, and then revolved a circle (like a wire ring) joining all the block together again. No problem.

Thanks for the explanation, I figured that out just before I closed my laptop for the weekend

Looks like an unfortunate limitation. I assume the only way around it is to come up with different methods for modeling the same geometry.

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