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Clearly I'm confused on how to use sketch library
Josy_La
Member Posts: 82 ✭✭
It seems I don't understand the workflow required to be able to reuse derived sketches. I know I already asked the question, probably a couple of time even, but I guess the answer is not clear for our context. Maybe I'm trying to hard to imitate the workflow used on our current platform... who knows? I appreciate your patience in trying to make the process clear for me.
First I created individual libraries to organize our different type of information; imported fastener models, imported our standards shapes (cad dwg) which where inserted in multiple sketches, created machining sketches directly in OS. Up to this point no issues.
In a new workspace I included those libraries thinking it would make it easier to choose within current document rather than browse <<= Is this the proper way to do things in OS? I derived the fasteners library, this one is easy and always accessible in any part studio via derive feature. Where I'm having a problem is with the sketches...
1) If I copy-paste tab containing inserted dwg from library to current document the information is unlinked which is exactly the opposite of what I need.
2) Tried to copy-paste a tab containing derived sketches but I have errors because link to actual import information does not follow.
3) When I derived sketches from library into current document I cannot use them in another part studio tab since it is impossible to rederived within same workspace.
My feeling is that library concept I was thinking of is best used for parts; file can be derived and parts reused easily. While library of sketches should remain external and individually derived when needed. I would of liked being able to derive an entire sketch library workspace and insert derived feature in sketches like it is possible on other platform.
For us it is critical to link our product shapes to parts created due to design assist running parallel to fabrication process. Shapes can be modified multiple time during process and final product needs to adapt accordingly.
First I created individual libraries to organize our different type of information; imported fastener models, imported our standards shapes (cad dwg) which where inserted in multiple sketches, created machining sketches directly in OS. Up to this point no issues.
In a new workspace I included those libraries thinking it would make it easier to choose within current document rather than browse <<= Is this the proper way to do things in OS? I derived the fasteners library, this one is easy and always accessible in any part studio via derive feature. Where I'm having a problem is with the sketches...
1) If I copy-paste tab containing inserted dwg from library to current document the information is unlinked which is exactly the opposite of what I need.
2) Tried to copy-paste a tab containing derived sketches but I have errors because link to actual import information does not follow.
3) When I derived sketches from library into current document I cannot use them in another part studio tab since it is impossible to rederived within same workspace.
My feeling is that library concept I was thinking of is best used for parts; file can be derived and parts reused easily. While library of sketches should remain external and individually derived when needed. I would of liked being able to derive an entire sketch library workspace and insert derived feature in sketches like it is possible on other platform.
For us it is critical to link our product shapes to parts created due to design assist running parallel to fabrication process. Shapes can be modified multiple time during process and final product needs to adapt accordingly.
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Comments
That piece of advice over, let's see if i can help you.
What's not clear is why you are not following the simplest path - let's start there . . . .
1) To reuse a standard part in an assembly - use 'insert' and then 'Browse documents' to find the part (or assembly) that you would like to insert.
2) To reuse a standard part in a part studio - use 'derive' and then 'Browse Documents' to find part and then 'Transform-by-Mate-Connector' to position/orient
3) To reuse standard sketches, there are a couple of workflows -
(a) Use 'derive' and then 'Browse Documents' to find the sketch. This places an (associative) sketch on the same plane and same orientation as the source document.
(b) If the sketch needs to be used on a different plane (or different position/orientation), then 'copy sketch' (RMB over the library sketch) and then in the target part-studio/document, select the target plane/face and 'paste sketch' (this is non-associative)
(c) This is the most complex workflow, but combines the benefits of (a) and (b) above. The goal is to create an associative (derived) sketch that can be positioned oriented. Insert the desired derived sketch. Extrude the profile. Apply a mate connector to the desired face and to the target plane/location. Perform a transform-by-mate-connector to position orient. From there you can convert edges in a new sketch or just use the face or boolean the solid body into the new part
In addition to the above, e are working on additional workflows to streamline the reuse of library sketches.
I hope this helps.