best practices with modifying assemblies

[pejaer]

I have often need to modify assemblies, and I am wondering why and what the logic is, that most of the "part features" (ie extrudes, chamfering, etc) are not possible in the assemblies? I am guessing that it is deemed "not good practice" to modify a component or part of an assembly...but two examples:

1. I work with plastic parts and it is common for me to heat fuse 2 parts together. Some of the resulting geometry would be much easier to approximate using fillets or chamfers in the assembly.

2. Another example would be: what if you are making a part out of plywood (and need to show the layers). First step would be to create a sheet of ply-wood, second step, for example would be to make a 45 degree chamfer around the edge....can't do it, unless you make a cut (the only function that seems to be available in assemblies).

I am looking for both practical solutions (if any!) and also some insight for the reasoning SW is setup this way.

Thanks
Paul

 

[CorBlimeyLimey]

Cuts (material removal) can be made in assys. Extrudes (adding material) cannot ... although welds can be created, they are actually treated as separate parts.

I guess a chamfer is treated as a mod to a single part.

Configs of the assy condition of a part can be created at the part level and shown in the assy level.

 

[gwubs]

I agree that being able to chamfer or round an edge in an assembly would be nice. As it stands we need to use the more tedious cut methods.
Adding material in an assembly should never be possible because you need the material to come from somewhere - that makes it a BOM issue. Think of it this way, you can run a router around an assembled group of parts, sweep up the chips and dispose of them, but you cannot add material with out it coming from somewhere.
A quick point about fillets, Sw treats fillets and rounds with the same term and tool button, but they are not the same thing. A fillet is concave (material added) a round is convex (material removed)

 

[pejaer]

CBL: Yes, I am organizing the assemblies as you suggest; that is creating configurations in the upstream (raw mat'l) and using these part configs in the assembly. However, it can get complicated when you have multiple levels in a hierarchy of assemblies....one needs to always go back to the part level, but then (it seems) 90% of the time I need to create a configuration at each level of the hierarchy as it is carried through to the final assembly. If you work this out, put the model aside for six months and come back....takes some time to follow the maze. For what it is worth, I have been naming my configs with the downstream part number to try to keep it organized. I have not used welds, and perhaps that will help...thanks for this suggestion.

GWUBS: Thanks for the input; and I agree with your comment regarding adding mat'l in an assembly....the mat'l added should be a part such as adding rivets or glue when putting three subassemblies together, for example. I would say an extrusion is a bad example; and perhaps perhaps my question is limited to modifying parts in the assembly....in fact, I suggest mat'l should not be added, but more powerful tools for removal (fillets/chamfers) and also "shaping" is needed. In my heat forming example, material is not removed, it is repositioned (nothing added or lost). Sounds more like surface modifications in the assembly?

And quickly back to the "rounds" that you describe. It seems that one can use both practices; drilling down to the base part to utilize the easy fillet feature, or one can stay in the assembly and use the more cumbersome (or at least more time intensive) sketch and cut method. I have used both methods and it seems to me there is that gap in the SW program for a fillet/round function in the assembly. At least you have confirmed a similar desire.

thanks.

 

[bencollins]

From a philosophical point of view, the post assembly plastic weld operations are themselves a separate entity / process, and could perhaps be best represented by a new part, i.e. weld bead etc. With all the weld beads thereafter collected as there own sub assy.

 

[SteveMartin]

I don't know how complex you're talking for assemblies, but for heat-fusing two parts together I'd be more likely to make it as a multi-body part. This won't work (well) for all situations, but in the work I do anything that can't be non-destructively disassembled is a part - anything that can be disassembled is an assembly. Sometimes I have 2-3 base parts imported into a single inseperable final part (which may then have more machining). This trades one set of limitations for another, however, as the part move/mate interface for multi-bodies is less user-friendly than the same interface in an assembly.

 

[cpretty]

SteveMartin has it sussed. (I thought)

For the plywood example, a multibody part is likely the best way. That way you have discrete layers of plywood, but can use all the tools on them.

If it is super important to then see each layer on its own in its own part, then use the split function to split each body off into it's own saved file.

BUT - there is always a but it seems.
After trying it for an example I have hit upon a very similar problem. You can't put a radius on multiple bodies. This would be nice if you could, and to my way of thinking more suitable than being able to do it in assemblies.

The multibody method may help with other issues you are having though.

For my plywood example attached, I have made it of 3 layers of ply, which you can split out if you need exact shape of each layer, then combine (ie gluing stage of manufacture), then finish.

Cheers,
Craig

 

[gwubs]

cpretty - I had the same thought and ran into the fillet on multi body limitation too. Took a quick look, but could not see a feature scope type setting to include all the bodies within the fillet.

 

[mjcole]

One possible solution would be to use the insert part option on Features menu to place the part files together in a new part rather than Assembly. This will bring in any changes made to the original parts in the new one and if a Combine feature was used to join the Solids you could then fillet or chamfer them.

Insert Part has a launch Move dialog option that can be used to set Mating constraints between the inserted parts and other geometry.

Michael

 

[NomLaser]

I think the easiest way to accomplish this is to save the assembly as a part file once the design is complete. Then you can go back and add your fillets and chamfers. You will loose the ability to change them as an assembly but it shouldn't matter much if the design is complete.

 

[gwubs]

Many of the ideas offered above show the creativity of SW users, and on a case by case basis can be used to get through a project. Going back to the start of the thread, it seems clear that SW has no "nice" way to apply material removal steps like rounds, in an assembly. This means we need to keep filling out those enhancement requests. We do get new features in each release. Check out the beta program for what's new in SW2010. Can't elaborate, as we are sworn to secrecy when we join the program.

 

[NomLaser]

2009 was supposed to support different materials on multiple bodies in the same part file, but it ended in a flaming pile of failure.

 

[pejaer]

Thanks for all the dialogue. I will take a stab at DEddie's save as a part file method next....perhaps saving an assembly as a part and importing it back into assembly will allow the needed modifications while maintaining also a BOM (ie playing with configs and suppressing parts where appropriate).

Paul