I was advised to use a library feature instead of a forming tool in This post
But it seems I can not sketch pattern this library feature.
Am I doing something stupid again?
Both library feature and a sample file is attached.
Any kind of advice is much appreciated.
Why Solidworks fails to sketch pattern a library feature?
Why Solidworks fails to sketch pattern a library feature?
- Attachments
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Part11.SLDPRT- (115.73 KiB) Downloaded 55 times
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- HalfShear.SLDLFP
- (129.24 KiB) Downloaded 72 times
That works, but you can also change the library feature so that a single sketch will work. The root cause seems to be the fact that the extrude sketch and the cut sketch are on the same plane. If you change the library feature to do the extrude first, and then use the end face of the extrude for the cut sketch (using Offset of course), the pattern will work using a single sketch:mike miller wrote: ↑Wed Oct 13, 2021 1:13 pm I tested it, and it is fine as long as your sketch locating the library feature is separate from the sketch used to pattern. IOW, you'll need two sketches: one to locate the feature, and another to drive the pattern.
This has nothing to do with library features by the way. You can dissolve the library feature and you will have the same problem.
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mattpeneguy
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Re: Why Solidworks fails to sketch pattern a library feature?
Sorry, it's a future version file for me. So, I can't help.
@HerrTick, @gupta9665, @jcapriotti any of you have time for this?
@HerrTick, @gupta9665, @jcapriotti any of you have time for this?
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jcapriotti
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Re: Why Solidworks fails to sketch pattern a library feature?
I don't have 2021 installed.
@Tera You are inserting the library feature, then doing a sketch driven feature pattern after?
@Tera You are inserting the library feature, then doing a sketch driven feature pattern after?
Jason
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mike miller
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Re: Why Solidworks fails to sketch pattern a library feature?
I tested it, and it is fine as long as your sketch locating the library feature is separate from the sketch used to pattern. IOW, you'll need two sketches: one to locate the feature, and another to drive the pattern.
He that finds his life will lose it, and he who loses his life for [Christ's] sake will find it. Matt. 10:39
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zxys001
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Re: Why Solidworks fails to sketch pattern a library feature?
Per Mike... it works. You can't share the same point you had.. it piled on the feature on a feature. (image)mike miller wrote: ↑Wed Oct 13, 2021 1:13 pm I tested it, and it is fine as long as your sketch locating the library feature is separate from the sketch used to pattern. IOW, you'll need two sketches: one to locate the feature, and another to drive the pattern.
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"Democracies aren't overthrown; they're given away." -George Lucas
“We only protect what we love, we only love what we understand, and we only understand what we are taught.” - Jacques Cousteau
“We only protect what we love, we only love what we understand, and we only understand what we are taught.” - Jacques Cousteau
Re: Why Solidworks fails to sketch pattern a library feature?
That works, but you can also change the library feature so that a single sketch will work. The root cause seems to be the fact that the extrude sketch and the cut sketch are on the same plane. If you change the library feature to do the extrude first, and then use the end face of the extrude for the cut sketch (using Offset of course), the pattern will work using a single sketch:mike miller wrote: ↑Wed Oct 13, 2021 1:13 pm I tested it, and it is fine as long as your sketch locating the library feature is separate from the sketch used to pattern. IOW, you'll need two sketches: one to locate the feature, and another to drive the pattern.
- HalfShear-Patternable.SLDLFP
- (129.56 KiB) Downloaded 56 times
Re: Why Solidworks fails to sketch pattern a library feature?
I really appreciate everyone's help.
Million thanks.
Million thanks.