Reference to another assembly

3D Design Volume Model
1

Good evening

 

I often have to constrain parts located in one assembly to an element in another assembly, except that when we try this operation we get the following warning:

"Please select inside the subassembly you are editing for the constraint"

 

Currently, I am trying to orient my tubes (see PJ) parallel to the blue axis which is the axis of the forestay of my boat and which is therefore part of another assembly (that of the rigging).

I don't want to create a new axis because I need the two to be linked, if the angle of the prop is changed, the tilt of my tubes needs to be as well.

More generally, I am often confronted with this problem, especially when I want to position the front of a piece of furniture (located in the sub-assembly of the furniture) on a partition (located in the "partition" sub-assembly) and that obviously I only want to move the front and not the whole furniture.

 

Has anyone ever been in this situation?

 

Thank you very much,

 


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Make subassemblies Flexible instead of Rigid

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We have to work with plans and constrain these plans

And it is this plan constraint that will make it possible to position these pieces

@+ ;-)

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That's exactly it =), thank you Alain.ERP

 

For those who might be wondering, this is what a Flexible/Rigid assembly is:

 

http://help.solidworks.com/2016/french/SolidWorks/sldworks/c_Flexible_Sub-Assemblies.htm

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Flexible sub-encembles are very practical but very heavy for SW.

From experience, they have become forbidden in our blends.

We had big problems with cons always in red, assemblies that were permanently over-constrained and constraint bugs.

FYI:

Flexibility is not recognized in lean assemblies.

If the assembly becomes overstressed for no reason, it must be switched to rigid and re-ironed to flexible.

It allows SW to recalculate the constraints (while it doesn't necessarily work with a CTRL+Q or a green light)

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It actually works well in the assembly, but the part comes back to its place when I open the subassembly to make a drawing.
Once the part has been constrained according to a reference of a parent assembly, is it possible to fix it in the position?

 

If I return the assembly state to rigid, the part returns to its original position, as does if I open the assembly.

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Pascal , so how do you use a partition located in another assembly to position a part?

Are there other methods that would allow you not to get an error?

 

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Basically, we don't make assemblies of rigid parts (physically in reality) between them.

For cylinder or hinge type assemblies, we work with configurations.

In some cases, a coin or envelope is inserted to hang on.

In other cases, the dimensions are simply transferred from one assembly to another.

If you can't do otherwise, you use the flexibility to define the position and then freeze it (it can lead to colision, but you ignore it)

We also sometimes insert the component twice (in the case of transmitter/receiver sensors under a single reference) and hide the part that is excessed.

These solutions depend a lot on the context of the assembly.

It's difficult to tell you how to do it without knowing much more about the architecture of your assemblies.

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