creating solids stead of cuts in assembly

[2ms1]

I would like to create some solid features (ie add material not remove it) in assembly mode. Whenever I try, however, the feature is automatically set to remove material. For example, this was supposed to be a cylinder of material added to what you already see in the picture. Instead, it came out as a cut:





Why would this be happening? I hope what I'd like to do isn't fundamentally impossible. When I create a new assembly with nothing in it I seem to be able to create whatever I want, but here I'm only able to create cuts.

 

[2ms1]

Ok I've decided that, at least with default settings or whatever, it is only possible to remove material by creating features in assembly mode. This is because whenever I try to create any kind of thing like a basic extrusion in anything other than a blank assembly file, the result is a cut/remove material.


Is there any way whatsoever to change this so I can add things like the little cylinder (outlined in red) as a solid rather than as a cut? My whole strategy to modeling this thing is screwed ifnot.

 

[paulgress]

I'm afraid to say, this is the default way pro-e works. In assembly you cannot create an extrusion.

I guess it boils down to the real world. You add parts to the assembly, then if required you do an assembly cut. This is usually called a "matched set" drawing or "secondary machining".

If you need to add that cylinder, add it to the existing part or create it stand alone and add it to the assembly.


Edited by: radelectronics

 

[csusie]

Have you ever considered creating a part, assembling
that part, activating it, and then creating the solid
feature. By activating the part, features will be added
to it rather than the assembly.

Have you used the command "activate"?

 

[Guru.hm]

what csusie is saying is correct..
u need to activate the part to add feature to it..

 

[2ms1]

Well, I was actually using that right there just as really simple example. What I would actually like to do though is add "pipes", basically, that connect a bunch of different things in the assembly. It would be very hard to draw the pipes without having the parts they run between all together to use as references... certainly very hard compared to just doing it in assembly. Would definitely be royal pain in ass... The piping all needs to avoid other parts in the assembly, hug along others as closely as possible, etc.
Edited by: 2ms1

 

[dr_gallup]

You can create protrusions to PARTS in the context of the assembly. Just not to an ASSEMBLY itself. Read the above posts. Activate the PART you want to add protrusions to and have at it.

 

[dgs]

Have you tried Pro|Piping? If you've got the Advanced XE package, you have it.

You could also toggle it from solid to surface and it will at least 'look' solid. I've used that to build wiring harness assy's.

 

[2ms1]

No I haven't, but I definitely want to learn it now. But all I seem to be able to find on the internet are books I would have to order and have arrive in a week or something. Do you, by chance, know of any kind of tutorials I could get somewhere right now? I need to start learning, like, tonight (for deadline)!

 

[dgs]

I checked and we don't have anything. This is one area that I'm not familiar with, though others here have used it successfully.

 

[[-Skint-]]

2ms1, hopefully you are well on your way with this now ? What you are lucking to do, is create the piping using all existing parts as references, what your are experiencing is that you cannot do this in assy mode, but after activating your new piping part in assy mode you will still be able to use the existing parts for reference.

 

[kdem]

Since you don't have Pro|Piping, you might want to try using a skeleton to pass geometry references to the part or parts that will be the pipes.

 

[2ms1]

I actually haven't found any tutorials and have basically just decided to make things with datum curves, sweep protrusions, and sweep cuts of smaller diameter to create the hollowof the"pipes". I don't need fittings and stuff like that anyway.


The thing that's a problem is that I need to know where the parts are located relative to each other in assembly in order to be able to create the "pipes". However, I can only create the parts of the piping that are integral to major parts of the assembly when I am in part mode and cannot see what I'm doing relative to the other parts. It's sorta catch-22-ish.


If I could create the parts in assembly mode then there wouldn't be any problem. It's the fact that you can only create cuts in assembly mode the creates the pickle.


Anyone have suggestions? What is this "skeleton" stuff you mention, kdem?

 

[kdem]

A skeleton is a framework for the assembly. Take a look in the Help under Assembly>Top Down Design>Assembly Skeletons to get started. You can define interfaces, mounting locations, etc. and pass the information down to the parts. In your case you may be able to setup a skeleton that contains the start and end points of the pipelines and any intermediate points you may need for pipe segments. There is a Top Down Design tutorial on the PTC website in the tutorials section that has an example of a skeleton. Not sure how much help it will be but it may give you some ideas.

 

[dross]

You CAN create parts in assembly mode.


Go to "insert > component > create"


Give it a name.


Click on "create features"


To later add protrusions to this part, click on it in the model tree while the assembly is open, right click and then "acitvate", you can then do whatever you want to it. This allows you to build a part in assembly mode using assembly references.