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Weird Cut Extrude

Question asked by Patrick Davis on Feb 14, 2018
Latest reply on Feb 15, 2018 by David Matula

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Again I'm having a problem, but in this case I've never seen this before or know how to fix it. I'm trying to do a regular straight cut extrude through my part and it is making odd points were it shouldn't or I couldn't cut everything because the program gives me an error saying it will result in zero thickness. The picture and model show what I can cut, but the pattern should be the same throughout the part which it isn't letting me do. I've made similar parts like this before and never had this occur in any of them. Does anyone have an idea on how to fix it? Thank you for the help and if there is anything else you need from me please let me know.

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138-1000-1 Right Side Flat.SLDPRT.zip16.6 MB

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Jay Hagan Feb 14, 2018 1:55 PM
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If you do a check prior to the cut it shows an error. Could be the problem.
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- Patrick Davis @ Jay Hagan on Feb 14, 2018 4:30 PM
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  Thank you for the reply. The check does show that I have a problem in that area, but it doesn't help me with the cuts through the part that aren't straight. I understand it has to do something with the transitions between the lofts I used to make the part, but don't understand why it is happening now and not before.
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  - Paul Salvador @ Patrick Davis on Feb 14, 2018 4:47 PM
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    Hello Patrick,.. if you rollback before the shell.. your min radius of curvature is ~.048".. and your shell is .09"...so, somehow, SW allowed this (blue offsets, bad).. and the geometry it has created is not good... so unfortunately, you'd need to clean the outer geometry to get clean inner geometry. (image attached,,.. also, turn ON VOR (verification on rebuild.. that is why you did not see the "exclamation error icon" on the shell).. the fastest workaround.. is to delete/replace/repair the blue surfaces)
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Glenn Schroeder Feb 14, 2018 4:42 PM
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Patrick,

I'm at home right now and don't have access to SW here, but I'll try to help. Are you trying to make all these cuts in one feature? If yes, is it possible that all the areas aren't selected at the bottom of the Feature Manager?

And again, if yes, did you use sketch patterns to reproduce any of the sketch entities? I (and many other experienced users) avoid them like the plague. It looks like the shape on the left worked okay. I'd suggest deleting the other sketch elements and try linear patterning the cut extrude feature. That often produces better results. Again, I wish I could open your model, and I apologize if I've made false assumptions.
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- Patrick Davis @ Glenn Schroeder on Feb 15, 2018 7:39 AM
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  Glenn,
  
  Thank you for the reply. The answer is yes to everything you said unfortunately. I first had a single sketch which cut through the part with no problem at all, then I did a linear pattern of the cut and that is were SW gave me the error of the result of end up having zero thickness. After that didn't work I tried a sketch pattern and cut everything singularly to find were I had the problems and the result is at the top. I uploaded the latest model which has the linear sketch pattern. I have also tried doing a loft cut to no avail.
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  - Glenn Schroeder @ Patrick Davis on Feb 15, 2018 8:20 AM
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    I don't know why linear patterning the feature didn't work for you. I opened your model, edited the sketch making all the linear pattern entities construction lines, and then linear patterned the feature without any problems. I'm using SW2018, so if I posted the file you wouldn't be able to open it, but here's screenshots of the result, and the Feature Manager.
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Tom Gagnon Feb 14, 2018 4:46 PM
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When I encounter a similar ZTG error, I find the tangent entities in my extrude sketch, and define it as 0.001" away from it instead of on it.

Then again, I don't manufacture typical parts. My business buys parts and assembles them. Therefore, tiny erroneous details within a part matter little to me.
That is, I think that others with more demanding feature tolerance will have a better answer.
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David Matula Feb 15, 2018 9:36 AM
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patterns are the key to multiple same cuts. sketch pattern or a feature pattern. think if you get done with this whole thing and someone decides to change the shape of those holes. I have worked on models before that trying to find the feature to change is difficult at best if not just plain frustrating. Then when you get to where they created it to make the change it ends up making multiple changes to everything else that does not need to change. Many a time I have taken a 96 feature part and turned it into 2 to 3 features but you are not sure when making the first part how best to proceed you do what you know and what your told to get something for people to look at. Then once you have a good picture, of what they want it may be time to start over to simplify and make things more user friendly.
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Weird Cut Extrude

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