CAD Forum

I have a part that is a pseudo assembly with individual parts placed within it. Some of the parts have broken references. The specific error is "out of context". But it also says it can't find the original part when I try to edit it.

I thought I found how to edit the references but it won't let me actually change anything. Hopefully I've provided enough information on how to fix these broken references.

Sorry, just noticed I didn't actually ask a a question...How do I update the references to sub components that were placed into a part?

This shouldn't be this difficult.

I can Right-Click on the part in question (a weld cap), then select "External References". This SHOULD be where it can be edited. It is even implied by the Lock button which PREVENTS reference editing until unlocked. But if I select on the reference in the "Part" field the filepath is not editable.

I think that it kind of depends an how the references were referenced.

Is it part in part reference?
Is it sketch references from a different part in the context of an assembly?
Is it part references in the context of an assembly?

As my thread title states...part in part

I think I found the right spot but I can't actually edit anything. Usually this means I haven't done the correct order of secret clicks in order to "enable" editing but I haven't stumbled upon it yet.

Problems like this are why I never use part in part.

Are you saying its broken/doesn't work?
I used part in part because the "assembly" is actually a welded part and not an assembly at all. Seems like the usage case for this type of idea. But, I'm beginning to see your point though.

Broken probably isn't the correct word.

But locating a part within a part only has a few options, compared to locating a part in an assembly. Plus you can drag parts around in an assembly where you can't with a part in a part. Like you have found, you can't open the part from the part for editing.

I come from a background where mutlibody parts didn't exist, and my experience with Solidworks has convinced me to avoid them as much as possible. (In NX parts and assemblies are the same thing.) Other people use them extensively, but they don't work for my workflow. I also don't use weldments, structured systems or sheetmetal, which is where most people use part in part. (I'm not philosophically opposed to those tools, they just aren't needed for what I design.)

SPerman wrote: ↑Thu Feb 10, 2022 3:52 pm . . . I come from a background where mutlibody parts didn't exist, and my experience with Solidworks has convinced me to avoid them as much as possible. (In NX parts and assemblies are the same thing.) Other people use them extensively, but they don't work for my workflow. I also don't use weldments, structured systems or sheetmetal, which is where most people use part in part. (I'm not philosophically opposed to those tools, they just aren't needed for what I design.)

Multi-body Parts in SW works great. Inserting Part in Part is a whole other animal.

Good point.

Glenn Schroeder wrote: ↑Thu Feb 10, 2022 4:02 pm Multi-body Parts in SW works great..........

Until:

-you want to reuse a body in other context
-you need to remove the part file at the top of a long tree (>1000 features, anyone?) or perform any major edit to the structure of the product
-you need to make a comprehensive BOM and sort by thickness, or anything that would move line items out of their respective subassemblies
-you need to make drawings for each part and discover that cutlist properties cannot be added to the sheet format
-you lose the lottery and have a huge part file that keeps corrupting its cutlist (we have one that corrupts on a regular basis)

So you decide to use Save Bodies to eliminate several of the above issues and discover that:

-gage tables must be defined AND MUST MATCH for the master and children (master defines bend radii and child defines flattening and K-factor)
-Save Bodies is next to unusable with configurations
-derived patterns don't work because it's dumb geometry
-rebuild and save times climb out of control



It might be okay for some applications, but not for most people.

jmongi wrote: ↑Thu Feb 10, 2022 3:38 pm I used part in part because the "assembly" is actually a welded part and not an assembly at all. Seems like the usage case for this type of idea. But, I'm beginning to see your point though.

There's no rule you have to use a Solidworks assembly file to model an assembly or a rule you have to use a Solidworks part file to model a part. They tend that way, but often don't match up. We use a part file to model a commercial off-the-shelf assembly. We use an assembly file to model sheet metal with inserts and other such parts.

We also find that a part-in-part model can have its troubles, but they have their place when nothing else will do.

Dwight

This has been an interesting discussion on part in part/multi-body....but...is there an answer to my original question? When I get to the area where it appears I should be able to edit the references, I cannot. Has anyone updated a reference in a part in part situation? Is it a bug that it doesn't work? Is it user error? Something in-between?

jmongi wrote: ↑Fri Feb 11, 2022 8:11 am This has been an interesting discussion on part in part/multi-body....but...is there an answer to my original question? When I get to the area where it appears I should be able to edit the references, I cannot. Has anyone updated a reference in a part in part situation? Is it a bug that it doesn't work? Is it user error? Something in-between?

OK, yes you can do it.
You cannot do it with the part open though.

Close the part, go to file-->open. Then select the part in your open window.
Once selected, click on the "references" button.
From here, you can double click on the name and select a new part to reference.

Thanks! That worked.
I must not understand SW nomenclature. Like what is the difference between a broken reference (what I thought I had) and an "out of context" reference (which is what it said I had).
It's a bit counter-intuitive to me that after I see that there are reference issues when a part is open that i have to CLOSE the part and half-reopen it in order to fix the missing reference. Oh well.
Thanks Dan1

jmongi wrote: ↑Fri Feb 11, 2022 9:47 am Thanks! That worked.
I must not understand SW nomenclature. Like what is the difference between a broken reference (what I thought I had) and an "out of context" reference (which is what it said I had).
It's a bit counter-intuitive to me that after I see that there are reference issues when a part is open that i have to CLOSE the part and half-reopen it in order to fix the missing reference. Oh well.
Thanks Dan1

I think that "out of context" just means that you don't also have that part loaded in memory.

If you select "All" in this area of your options, then you shouldn't have that problem.

Edit: After looking into it, "out of context" also means that geometry may have changed and Solidworks cannot find the geometry it was looking for.