Constrain the Sketch from One Component to Another in the Assembly (SolidWorks)

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1

Hi all

I try to make a protective bellows and then add it to an assembly of a machine. The problem I have is whether I can stretch it or not by modifying the sketch followed by an update of the assembly so that the two components re-coincide but I would like to know if it is possible to have this compression/tension movement just by moving one component relative to the other without having to go through the sketch.

Thank you in advance.

 


soufflet_2.1.png
2

Hello

The only solution I can see would be to make the whole bellows in assembly with distance constraints so that it can move in this assembly and then when you put it in the other assembly you will have to make it flexible so that it follows the rest.

3

Do you mean breaking down the entire flexible part (black) into several components and then putting them together?

Otherwise for the moment I have found an alternative solution but not perfect, as soon as I move component 1 I just have to update the assembly (without touching the sketch) so that the bellows adapts to its new configuration.

4

You have to edit the sketch in the context of the assembly, add coincidental/collinearity relationships.

However, be careful, this means that your bellows is dedicated to this ASM.
As I imagine that you only have a few positions, it seems to me wiser to make configurations in the asm and the room.

1 Like
5

See this link

 

https://www.lynkoa.com/forum/modélisation-volumique/répétition-selon-courbe-sans-normale-à-la-courbe

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6

I managed to constrain the sketch to another component, but now I have another question: is it possible that the position update is done automatically?

The bellows does not automatically follow the movement of the carriage to which it is attached (see image), it returns to the correct position only after the assembly has been rebuilt.

I hope my explanations are understandable


soufflet_na.png
7

Do you have to constrain your sketch correctly

you constrain the bellows on a parallel without the side 

Your parallels will be reserved if you stretch your fixing flanges

and the opposite if you reduce the eca Flasks 

So in your basic sketch

you must constrain the extremities on a line

and the bellows tips on another

The only dimension  next to it is the length of a side due to the triangle especially not the angles to allow the sliding 

@+

 

8

This is one of the problems of linked parts, it requires recalculating, sometimes several times, the model so that the situation is frozen.

9

The solution is either:

- to have a part with external references that rebuilds automatically according to the assembly (warning: it doesn't work if on a drawing you have several views with different part geometries)

- make length configurations in your flexible room and assign the right length to each configuration: it's heavier but cleaner. This is what we use for O-rings (flexible parts with a single purchase reference / bill of materials but several shapes possible depending on their assembly).

10

Thanks to you, I don't have too much time for the moment to look at it again, I'll stay with what I was able to do but I'll try again later.