Turning an Assembly into a part

You...could...use the Join Command. This takes an assembly and joins it into a single part...BUT all parts in the assembly must touch or interfere. Usually, there are some problems with using the join command. BESIDES, this will not really speed up your model anyway. In fact, it will most certainly slow it down.

My Suggestion: If you just want a way to insert this gearbox assembly into another assembly with a minimal performance hit, I suggest using a simplified configuration. Just make another config of your gearbox assembly that suppresses all unnecessary stuff. Then insert that simplified config into your new assembly.

Nathan,

Check out the "join" feature in the help section. I think is what you are looking for. You can take any assembly of parts and "join" them into one part. The joined part is fully associative to the original parts.

Hope this helps Rob

You can also do a File-> Save As on the Assembly and Select part from the File Type Pulldown. This will let you save a n assembly as a multi body part file.

Todd

If you want a little assistance with joining, I can send you the article I wrote on the subject. Let me know.

WT

But this is not associative with the original assembly file. If the assembly changes, the 'Save As Part' file will not update.

It does provide a nice performance boost, however.

We added a script to our PDM that automatically creates the Part from the Assembly to solve the synchronization problem.

Hmmm. Interesting idea. I am curious, though. If you use the 'Save As Part' in another assembly and mate to it, do the mates loose their references when another version is 'Saved As Part'?

You should be able to do a "Replace Part" or perhaps even ovewrite the old file with the new. Broken mates will probably be an issue depending upon how many topographical changes were made. The "Repair Mate" tool is pretty good though.

JJ

The references remain intact - unless you do something to that feature that would break them anyhow. When you save an assembly as a part, you wind up with all of the former parts as distinct bodies in the assembly. Those bodies retain their features, so there aren't any problems with mating. You cannot, however, replace the assembly with the part (or vice versa) and have the mates work out.

Using the save as assembly as part route, obviously any changes in the assembly are not reflected in the part file unless a macro is used to keep the part file up to date as suggested by Gabe. However I find that the mates can broken to a point where they are difficult to diagnose occasionally.

What would be nice is if a face could be give a unique name that will remain constant regardless of other changes to the model (provided the face in question is not altered). Now this is possible using the 'RC/Face Properties/Entity Information' box but this seems to have no effect on mates.

A new idea I am going to trial (as time permits) is to create 0 offset surfaces of critical features, (bosses, holes, etc which will be used in the assembly for mating purposes). Then hopefully applying mates to the surfaces rather than the solid faces will allow mating surfaces to be preserved regardless of any changes to the model. This of course relies on the 'hope' that the surfaces won't be renamed... okay I'm probably clutching at straws.

Regards Iain:-)

Iain,

A word of caution.... I have played with using surfaces in the same way. The biggest drawback I found with them is if you ever want to use those surface models in a drawing. SW won't play well with surfaces in drawings. Try to create a dimension in a drawing to a surface (not a face), and you'll see what I mean. I have gotten it to work before - sort of - by creating sketch segments to represent the surface that the dimension would reference, but it is a REAL pain.

I've still haven't decided on what I should do, I've been doing alittle bit of playing around. The one problem I am having is when I insert the assembly with the sub assembly of my weldment into a drawing and I create a section view, my case is hatched as different parts and you can see all the different parts of the sub assembly (weldment).I want it to look like all one peice hide lines all hatched the same. I run into a similar problem when I create a part from my weldment assembly, the cross hatch is right but I can still see the line where my parts join in my assembly. The line wont goaway when I RMB "Hide Edge"

Thanks for all your help guys

Nathan Feculak

Offset surfaces can get broken pretty easily. I have tried this, and moved away from it.

Wayne,

If it's not too much trouble, I would love to read what you have on joining, as well.

Sincerely, Jerry Forcier

Wayne Tiffany wrote:

We design mobile mining equipment and a majority of our assemblies are fabricated and than machined. The machining operation is a configuration that uses assembly cuts. This method works well for us and theres no noticable slow down caused by using assebly cuts. We prefer this method because it keeps the designer focused oh how the assembly is actually made and less on how to work around the system.

This is curently what I do as well but the problem that I have is when I section the view my sub assembly of my case looks like 10 different part and I need to show it as one. For some reason when I try to hide lines they wont hide, and I would like to crosshatch them as one peice.

To change all components in an assembly section view to the same hatch. Right mouse click on a cross hatch select properties, pick a hatch style, and select apply to "view" this will change all components to the same hatch.