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Subdivide an element
baumar
OS Professional Posts: 77 PRO
Hi,
I have several elements in my drawing that I would like to subdivide in equal subelements. I created a sketch showing the whole element and the goal that is the element composed of subelements ( the size of the sub elements is not equal, but will have to be in the real subdivision).
Does anybody knows a smart way to do that? If there isn't a standard function I ignored so far, would there be a feature that does the job?
Thanks for help
Markus
https://cad.onshape.com/documents/6241cb432116d5696cd40a02/w/08ce71397dea0649f2c253e5/e/4b780ac1d0be3266e6b2eb6a
I have several elements in my drawing that I would like to subdivide in equal subelements. I created a sketch showing the whole element and the goal that is the element composed of subelements ( the size of the sub elements is not equal, but will have to be in the real subdivision).
Does anybody knows a smart way to do that? If there isn't a standard function I ignored so far, would there be a feature that does the job?
Thanks for help
Markus
https://cad.onshape.com/documents/6241cb432116d5696cd40a02/w/08ce71397dea0649f2c253e5/e/4b780ac1d0be3266e6b2eb6a
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Best Answers
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baumar
OS Professional Posts: 77 PRO
Thanks for the hint. Just one follow up question. I have to split an extrude into 40 subparts.
is there a way to separate it easily (that is without creating 40 planes and splits) into 40 subparts? Maybe there is a function or a feature script from someone who had the same demand?0 -
Jake_Rosenfeld
Moderator, Onshape Employees, Developers Posts: 1,646 
Hi @baumar ,
To answer your question to the best of my ability: Variables exist within the context of one part studio, they are not global to a document, and therefore cannot be used in an Assembly or a Drawing. Variables can be used in all input boxes of a part studio (with a small few exceptions). Variables are just features of a part studio, so they act like all other features with respect to our parametric system; namely, you can only use a variable in a feature that is after the "Variable" feature that defines the variable you're trying to use. Variables are always referenced as #variableName.
https://cad.onshape.com/help/Content/variable.htm
There should definitely be a variable feature in your part studio. It looks like "(x)". If you are using a small screen, it may be hiding in the second-to-rightmost dropdown:
Jake Rosenfeld - Modeling Team5 -
Jake_Rosenfeld
Moderator, Onshape Employees, Developers Posts: 1,646
@baumar
You can bring the entire Part Studio into the Assembly at once by clicking the Part Studio in the import dialog instead each part individually. Then, you can use the 'group' mate to ensure they stay locked relative to each other:
https://cad.onshape.com/help/Content/mategroup.htm
Does that help?Jake Rosenfeld - Modeling Team5
Answers
is there a way to separate it easily (that is without creating 40 planes and splits) into 40 subparts? Maybe there is a function or a feature script from someone who had the same demand?
This is the kind of thing that our 'Feature pattern' is for. I've made you an example doc showing how to slice an extruded piece 40 times:
https://cad.onshape.com/documents/bb912de1a3bb5eace5e4a9af/w/38f1a1db373548e870711bf5/e/e3a738a0358d34ebf0bcb9fe
You can copy this document and double click on the features to see their inputs. I made heave use of variables, so changing any of the variables at the top of the feature tree should change the model accordingly.
https://cad.onshape.com/help/Content/linearpattern.htm
https://www.onshape.com/videos/patterns-in-onshape-04-20-17
Just one little question: I searched where the variables that you defined will be used and I found by chance that clicking in the fields where the value appears that it is referenced with an # like #widthEach. so I can use any variable and use it anywhere in any item I guess?
Another thing I didn't get right is this: Even when I change the width to 50, the whole construction looks the same - though the distance is 5 times bigger. but just now I saw that you can obviously use the variable also in the drawing, is that right? That's awesome, because now you can give it a meaningful name instead of a 'meaningless' number
To answer your question to the best of my ability: Variables exist within the context of one part studio, they are not global to a document, and therefore cannot be used in an Assembly or a Drawing. Variables can be used in all input boxes of a part studio (with a small few exceptions). Variables are just features of a part studio, so they act like all other features with respect to our parametric system; namely, you can only use a variable in a feature that is after the "Variable" feature that defines the variable you're trying to use. Variables are always referenced as #variableName.
https://cad.onshape.com/help/Content/variable.htm
There should definitely be a variable feature in your part studio. It looks like "(x)". If you are using a small screen, it may be hiding in the second-to-rightmost dropdown:
Thanks for the hint, now I can use it, it's really a great feature*.
May I bother you with a follow up question: I now can make the elements that I need, but I end up with an 'opposite' problem: As I still want to construct the whole part (as it was before the splitting) - seen from my current knowledge - I have to add them to the Assembly one by one using the mates... time consuming and a bit monotonous.
I used a trick that I add the solid element in the Assembly first and split it afterwards in the part studio. This works from the point of view of look, but there is a kind of 'circular reference' between part studio and assembly which is not so good. Much more as I have to use the whole element several times in my design
It would be better to assemble the parts - in a hopefully easier way, where I would like to get a hint how to - then group it and reuse it in another assembly.
*I guess I will ask to have an option to display the logical name also in the drawing, in some cases I think that would make the drawing to be more descriptive. Would you agree?)
You can bring the entire Part Studio into the Assembly at once by clicking the Part Studio in the import dialog instead each part individually. Then, you can use the 'group' mate to ensure they stay locked relative to each other:
https://cad.onshape.com/help/Content/mategroup.htm
Does that help?
The beginning of this video shows how to bring in an entire Part Studio:
https://www.onshape.com/videos/assembly-mates
Thanks for the hint!