I am looking to insert an extruded profile into an assembly and adjust its length directly in the assembly using the other parts as a reference or limiting element.
Hello
I'm not sure it's possible, a solution would be to create a part and remove material in the assembly according to the other elements.
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A new part must be inserted to create an extrusion/boss. Unlike material removal, which can be done directly in the assembly.
Later, you can create volumes in the "assembly context".
If it's an nvolume that is not intended to have a plan (slddrw) you can put it in "virtual", it will then be saved in your assembly.
Hello
You just have to edit your part in profile and then your sketch which manages the profile in the assembly and hang the segments, the points on the other parts of the assembly !
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Otherwise, another solution is to use the part families, and create a family for each desired length.
Because if there is only one configuration and this part is used in another assembly, the length will not be good!
More information about the part families:
http://www.lynkoa.com/search/famille?type[0]=tutorial
In an assembly, you can do material removals, but not extrusions.
You are forced to insert a piece that uses your profile.
You create a room with your extruded profile.
You position it in your assembly to have the start of your extrusion in the right place.
You edit your part in the assembly.
You use an element of the assembly as a condition for the end of your extrusion (plane, face, point, line, depending on what suits you)
You have to see the conditions, but personally I don't recommend this way of doing things.
If your assembly moves, your part automatically updates but the associated drawing does not update until it is rebuilt.
If, in addition, your part is used in another assembly, it can cause a lot of problems.
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Hi @ C.Poirier
Post an image of your assembly
to know what type of ref will be taken into account to see the ins and outs
insert new parts
if you create planes on the contact faces
and a sketch in the center of these shots
You must be able to extrude on both sides of this sketch to the referenced plans
the problem you'll have afterwards
it's the constraints that depend on your support surfaces
@+.....................
Hello
For your profile, use (in component edit mode):
- or sketches constrained to entities of another component
- or by choosing, as a condition for the end of the extrusion function, a face or another entity of another component
Kind regards
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Hello.
I am a new user of solidworks after having worked several years on topsolid, and I was looking to find this function that I used a lot before. I see that it does not exist.
However, "Pascal", your answer still gives me an interesting solution for some cases, even if it should be used with caution.
Thank you all for your answers.
Hello
Why do you say that the function does not exist when @Pascal gave you the solution?
Maybe you want something extra, like being able to fill in the length value when inserting your profile and have it point to a dimension taken from the assembly?
Or other things.
I worked 11 years on TopSolid V6 (1998->2009) and I don't see what could be missing in SolidWorks at this level.
@+
@Coyote:
I don't see what could be missing in SolidWorks at this level.
I think he just wanted to create a sketch and extrude it directly into the assembly (something impossible directly under SW)
@cpoirier:
In your assembly you can:
make insert/component/new part (it will create a virtual component that only exists in this assembly)
you edit this component
you create your sketch directly on the assembly element (or you create a plan that relies on an element of the assembly before, I find it cleaner)
You extrude your sketch down to an element of your assembly.
You will have a component dedicated to your assembly constrained and defined in the assembly without having a part file next to it.
This method has the same disadvantages as the other.
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@Pascal, @cpoirier wrote insert in an assembly....
So let's wait and see what he meant precisely because it's clear that between SolidWorks and TopSolid V6 there is a big difference, TopSolid V6 doesn't have the notion of a separate part and assembly file.
@+
In fact, Pascal's answer is the same as mine, but a little more detailed, it's true!