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Insert Part into a Part (Solidworks)
2

Insert Part into a Part (Solidworks)

Insert Part into a Part (Solidworks)

(OP)
Hopefully you guys can follow this.  It will be tough to describe it using text.

We like to insert parts into other parts, create configurations and then insert those specific configurations into "finished" parts... thereby attempting to reflect the various stages of machining/finishing/stocking that we do with our parts.

The strange problem I run into, is when you do an assembly using these parts... and you have other parts mated to them... everything is fine.

Except...

You do a save-as to a new assembly.  You take this new assembly and try to replace one of these part-inside-a-part-inside-a-part with it's "brother", in other words, a part that lived the same life, except at the end we activated a different configuration before inserting it into it's final [finished] part (we're talking about the only difference being annodizing.. where part-A is black... part-B is silver).

Anyway.. you do this simple "replace compenents" and you it gives you invalid mates for every single mate that had anything to do w/ that replacement part.

Here's where it get's interesting.

You can repeat all this, but don't do any part-inside-a-part-inside-a-part business... and nothing blows up; all mates remain in tact.

I guess - does anyone out there use this part insertion frequently, and if so, do you find it to be a robust technique?

- Jack

RE: Insert Part into a Part (Solidworks)

I understand what you are doing.  In the past I have done the "part-within-a-part" deal using assemblies and have separate parts that represent it in each operation of machining.
 

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RE: Insert Part into a Part (Solidworks)

If you insist on doing this, you will have to mate with the three primary planes.  The reason is that when you insert a part into another part, the faces are not really the same.  Sure, they are in the same location, but the ID or whatever is different because it was created by inserting external geometry.

The reason mating with the primary planes will work is because they are present in the part template, therefore they really are the same feature in all parts.

-handleman, CSWP (The new, easy test)

RE: Insert Part into a Part (Solidworks)

evolDiesel,

When changing the config of an inserted part, the "Replace components" option should not be used.

Instead, RMB on the inserted component and select List External Refs, then a dialogue box will open and a different configuration can be chosen. The mates should then be maintained.

 

cheers

RE: Insert Part into a Part (Solidworks)

The colour of the inserted part will probably not be carried into the active part though ...especially if you are running SW08.

cheers

RE: Insert Part into a Part (Solidworks)

(OP)
CorBlimeyLimey,

I guess I didn't explain myself well enough (this is tough thru text).

I have a part in an assembly.

This part is built of multiple layers of part-in-a-part-in-a-part.  Some of these layers (parts) are mutli-configuration (representing a tab drawing).

If I have another part, that was created using the same base part, but a different configuration... and there is NOTHING different between the configurations (other than config 1.. config 2.. etc)... when I go to replace the component with that other part... I can't maintain any mate that was associated to the first part (remember... these are parts created from the same inserted (seed) part.. and nothing has been changed.. no features or planes or sketches or anything has been created.

I'm telling you ... it's a bitch to explain this over email.

I would take some screen shots... but I think we have a solution.

Since we use PDMWorks... we finally figured out how to search for a configuration.

Now that we can locate a configuration in our vault... there's no real point to creating parts from an inserted part (that has the configuration).

Once again... I'm sure this makes no sense via text lol.  You'd only know about this if you were a violent offender of part-in-a-part... as we are ;)

Thanks,

- Jack

RE: Insert Part into a Part (Solidworks)

I think handleman hit the nail on the head.  The act of inserting the part into another part generates new faces.  Your final parts have different faces, that is why the replace boogers the mates.

Though it seems you already have your solution, I would be curious to try to use more configurations, such that the level 1 part has many configs, the level 2 part has many configs and the level 3 part has many configs.  It sounded previously that you have multiple level 2 parts and multiple level 3 parts.  The suggestion is to roll those in to configurations of a single part at a given level.  That way you are only changing configs at the assembly rather than replacing.

But ultimately, I think the best solution (the one you have selected) is to use derived configurations within a single part to represent your machining stages and finish options.

-Dustin
Professional Engineer
Certified SolidWorks Professional

RE: Insert Part into a Part (Solidworks)

Hi, Jack:

Whether you need to create parts ("DERIVED PARTS") from an inserted part is up to your design intent.  Derived part function is an important of any solid modelling.

Just like Dustin pointed out, when you insert a part into another part, you create a brand new part which has totally different vertex, edges, faces and volume IDs from those of the base part.  Same thing happens when you insert a part into an assembly.  The assembly may look exactly like the part, but it has totally different definitions in SW database.  That is also why replacing a part with an assembly will booger mates and views in drawing documents.

Alex   

RE: Insert Part into a Part (Solidworks)

(OP)
The (2) posts above this one really seem to spell it out for me.

It looks like no matter how "exactly the same" 2 parts are after they were created from the same seed part - solidworks still views them as mutually original parts and.. this is why even the most simple surface to surface mates, which look the same, don't work.

OK... thanks for the replies guys.  This was a good thread.

- Jack

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