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How to 'machine' an assembly?
Henk_de_Vlaam
Member, Developers Posts: 244 ✭✭✭
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?
Henk de Vlaam (NL)
1
Best Answers
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3dcad Member, OS Professional, Mentor Posts: 2,476 PROYep, 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 -
emagdalenaC2i Member, Developers, Channel partner Posts: 863 ✭✭✭✭✭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
https://cad.onshape.com/help/#in-context.htm?Highlight=in context
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/6aebbcff6889f0254d64e2a3
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:
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.
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.
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/19bdd39421cb04aa9576bcee
Eduardo Magdalena C2i Change 2 improve ☑ ¿Por qué no organizamos una reunión online?
Partner de PTC - Onshape Averigua a quién conocemos en común
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.
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.
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