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How to 'machine' an assembly?
Henk_de_Vlaam
Member, Developers Posts: 269 ✭✭✭
I like to make a cut in an assembly that intersects several parts. The parts come from different part studio's so that it is not possible to do a boolean operation in one part studio.
Has someone a suggestion?
Has someone a suggestion?
1
Best Answers
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Yep, assembly level cuts are needed - but we need two solutions:
1. Cut that is made in assembly just to get the hole position correct in all parts. When manufacturing hole will be machined to each part separately.
2. Cut that is actually made after assembly, does not appear in parts but will be shown in assembly.
For your current situation, could you edit in context part by part and sketch with 'use/project' tool to link hole position between parts.
Very quick example here https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/702ddcfb91bc58d2d9b8f8d1
Part studio is not important, parts can come from different studios but look at assembly in context features. I suppose linked docs cannot be edited in context as they are locked version - or does Onshape create new version on edit?
If you try this, remember that you need to update each context link to apply changes. Should be easier than positioning derived parts.
If picture shows the real situation, I would go with single studio that let's you 'drill' with single feature through all parts.
//rami10 -
There are an easy way...
1- In the Assembly. Create a NEW in context part.
2- Use the transform feature with the option Copy in place and select all the parts that you want (you can select with a rectangular capture all the parts of the roof that you want to cut)
3- Create the cut extrude
4- Create a New assembly, and insert the parts or all the Part Studio.
You can check it here https://cad.onshape.com/documents/904d2a9d5e7d264f0b1c69ce/w/8bae942b532ef51921b05868/e/19bdd39421cb04aa9576bceeUn saludo,
Eduardo Magdalena C2i Change 2 improve ☑ ¿Por qué no organizamos una reunión online?
Partner de PTC - Onshape Averigua a quién conocemos en común6
Answers
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I'm not 100% sure what you are asking for but it seems that in-context modelling might be your friend...
https://cad.onshape.com/help/#in-context.htm?Highlight=in context
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@brian_jordan,
In the example you see two identical blocks/parts assembled/glued together. I like to drill a hole, identified by the red marked sketch, in this assy.
When I drill the hole as suggested by edit in-context, then I get the part like shown below which is not the solution I wish. To be clear: I do not like to see the hole segments in the part in the part studio.
For reference see: https://cad.onshape.com/documents/888da41ee74f5b788d05c4bc/w/81367712fdd18c359c14b441/e/6aebbcff6889f0254d64e2a30 -
I think in that case you have to use derived to bring the parts into another part studio. An assembly cannot modify part geometry.Ilya Baran \ VP, Architecture and FeatureScript \ Onshape Inc0
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@ilya_baran,
Sorry that does not make sense to me.
What I discussed here yesterday was just an example. In real life I like to make a hole into a roof. See picture below: the red marked hole in the green Through All direction in assy B.
This is what I think I have to do:- Create a new part studio A
- Derive all the part that are intersect by the virtual square hole into that studio and transform them to exactly the same position as in the assy B. That's a lot of precise work.
- Make the red sketch and intersect them Through All. See next picture.
- Remove in the assy the parts that were derived in part studio A
- Insert part studio A into assy B on the right spot.
Is this true? When this is the way to do things up till now then a enhancement should shine at the horizon.
So I voted for https://forum.onshape.com/discussion/1334/assembly-level-extruded-cut-feature.
That is the enhancement that I like to have because it is what happens in the real world.0 -
Yep, assembly level cuts are needed - but we need two solutions:
1. Cut that is made in assembly just to get the hole position correct in all parts. When manufacturing hole will be machined to each part separately.
2. Cut that is actually made after assembly, does not appear in parts but will be shown in assembly.
For your current situation, could you edit in context part by part and sketch with 'use/project' tool to link hole position between parts.
Very quick example here https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/702ddcfb91bc58d2d9b8f8d1
Part studio is not important, parts can come from different studios but look at assembly in context features. I suppose linked docs cannot be edited in context as they are locked version - or does Onshape create new version on edit?
If you try this, remember that you need to update each context link to apply changes. Should be easier than positioning derived parts.
If picture shows the real situation, I would go with single studio that let's you 'drill' with single feature through all parts.
//rami10 -
There are an easy way...
1- In the Assembly. Create a NEW in context part.
2- Use the transform feature with the option Copy in place and select all the parts that you want (you can select with a rectangular capture all the parts of the roof that you want to cut)
3- Create the cut extrude
4- Create a New assembly, and insert the parts or all the Part Studio.
You can check it here https://cad.onshape.com/documents/904d2a9d5e7d264f0b1c69ce/w/8bae942b532ef51921b05868/e/19bdd39421cb04aa9576bceeUn saludo,
Eduardo Magdalena C2i Change 2 improve ☑ ¿Por qué no organizamos una reunión online?
Partner de PTC - Onshape Averigua a quién conocemos en común6 -
@emagdalenaC2C,
Thanks for the idea of Copy in Place. However, it's still necessary to create extra assies. So, I'm still looking forward to assembly features.0 -
i think i am in the right concept of a thread.can anyone help me with my document?i would like the ends of the DC connector to be limited by the board under clearance so it does not show up. the part does have them that long but after soldering they are cut. is there a way to show this in the assembly with out making the part itself cut off?
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I would suggest that this is an argument for constructing several related parts in one part studio as opposed to having one part studio per part0
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I would disagree on this,GWS50 said:I would suggest that this is an argument for constructing several related parts in one part studio as opposed to having one part studio per part
I created a part studio that generate alupanel board of any dimensions, you just have to give it the width, height, and thickness of the product that you need.
This has then all the correct part number, vendor and color for this product.
Then once this is inserted in an assembly, how do you make modification? (Hole for windows, screw).
This is valid for any product that you buy raw and need to make modification for each of your product, does not have to be a panel.
could be as simple as a small box that you buy and you have draw in you "database" of of the shelf product.
I don't want to have 25 boxes different boxes having all different holes placement depending on customer need.
This assembly modification is one of the thing that I really miss.
Is there a easy work around other then creating copies?
Thanks for all guys.
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@patrick_farley Maybe it's because I never figured out a reasonable robust workflow that did not involve constant recreation of assemblies, but I'd like assemblies to be deprecated and have the mate functionality pushed into the part studio. Assemblies just feel vestigial. If you want to pose your parts based on mate manipulations then have feature that lets you pose them.
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Thanks for the comment,billyzelsnack said:@patrick_farley Maybe it's because I never figured out a reasonable robust workflow that did not involve constant recreation of assemblies, but I'd like assemblies to be deprecated and have the mate functionality pushed into the part studio. Assemblies just feel vestigial. If you want to pose your parts based on mate manipulations then have feature that lets you pose them.
I don't think that assembly need to be deprecated, but I do like your idea of adding mate in part studio.
I added you some example of why assembly should still be needed,
In this example, i am designing a aluminum mounting plate that could hold a LCD display, an arduino and a keyboard.
I am only designing the mounting plate.
But all the other part are already drawn either by the manufacturer or a nice guy :-:smile: .
So I would not like to have to draw all of those part from scratch, an this is where the assembly is king
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@patrick_farley All of those parts could live in a partstudio. In fact if they were in a partstudio you could have them parametrically laid out and have all the holes cut out of the panel too.
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