assembly cut best practices

[housta]

Hi everyone,


I'm a long time IDEAS user, and relatively new to Pro-e (wildfire 2). I have used the assembly cut feature to cut my part. My question is this. I created a "cutter assembly" becauseI had to simplify my cutter part before I used it, hence the need for a separate assembly. I assume that if I delete that assembly, the relationship between my cutter part and my target part will be gone? I would like to get rid of the assembly as it is "extra". I'm used to IDEAS were this was done at the modelling level not assembly. Was this the best way to do this?


Thanks everyone, BTW pro-e kicks IDEAS arse!!!

 

[tommypurple2]

If you make a cut in an assembly it will always reference it. You can in the assembly right click the component in the model tree and activate it and then make you cut to your component. This will put the feature in the component model tree and not in the assembly model tree. So you will see it if you delete the assembly.


Once you delete your assembly you will open a whole new can of worms tho.

 

[jeff4136]

I'm not sure I'm following exactly but the 'best' way will probably
depend on whether or not you have(?) an AAX license. That info and
some elaboration on 'why the assembly?' will help someone determine
if there's a better way.

 

[[-Skint-]]

Thanks everyone, BTW pro-e kicks IDEAS arse!!!

Upgrade to WF4... its even better

 

[housta]

Hi Jeff,


It looks like we have AAX. My target part is insulation that surrounds the cutter part, but I couldn't use the real base part because it was too complex and wouldn't give me what I wanted. So I copied the part, simplified it, renamed it as my cutter, then placed that and my target part in an assembly. From there I did my cut, and it worked well. Unfortunately, now I have an assembly and cutter that are "extra".


I guess my question is can I delete the cutter and the assembly? In IDEAS you would just cut your target part with the cutter, then in the target part history tree you would have the cutter part history as well if you needed to update anything. At that point you could delete the cutter part as it wasn't needed anymore.


Thanks!!


Al

 

[jeff4136]

Ok, (sorta, ~think~ I have a rough idea). If you have (I don't)AAX you can use various Copy Geom / Inheritance / ??? features without having to create the references in an Assembly environment. That's what I'd look into, anyway.


(Actually, you ~can~, even without AAX, copy your simplified cutter part geometry to the target part (in assy environment), use it to cut the target and delete the assembly. You'll get a missing ref warning but everything will stay alive. I'd probably do that rather than making an assembly feature cut.)
Edited by: jeff4136

 

[mcgowanp]

Hey Al, Jeffs's bang on there. You can make a surface copy of the solid surfaces of the cutter part and copy and paste this surface into the parts in the assembley mode, You need to activate the part you want to copy into first and then do the copy paste operation. Once you have it in there you then suppress the part in the assembly or delete it. The new surface will stay as it is and regen fine but on your global ref view you will see that there will be some references missing.


I've made a wee video to help you out here and uploaded it on to youtube, someone else started doing this and I thought it was a really nice way of helping people without actually giving them the part modelled, until we get a video section in here that is... ... admin are you listening??!!


http://www.youtube.com/watch?v=JGUp2G3Kc-w


Paddy

 

[mcgowanp]

Hey Al, i meant to show also one last thing of how you might handle changes to the cutter part, in this other video.


http://www.youtube.com/watch?v=Brde2daS_Qg


Paddy

 

[fiebigc]

I would strongly recommend against referenceing parts from the assembly. I consider this a crude method for making parts dependent on each other. The more elegant method is for a master model created entirely from surfaces. The master model is then completely merged into each part file or you can publish selected geometries that are selectively imported into each model. The laterly method being the more modern approach but both are still valid. If you really want to excel at ProE you need to learn to do things the ProE way. Forget how other CAD systems work. If you try and force ProE to behave the same way that the CAD system you already know only leads to great frustration and impedes your progress.

 

[housta]

Paddy, thanks for the videos, that was awesome!!! I really appreciate it. A huge help. Thanks to everyone for your help and I do have to say after using proe the last few weeks, it is a very good package. It blows IDEAS away.


Thanks!!!


Al Houston


ATK

 

[pjw]

Hey Al, Jeffs's bang on there. You can make a surface copy of the solid surfaces of the cutter part and copy and paste this surface into the parts in the assembley mode, You need to activate the part you want to copy into first and then do the copy paste operation. Once you have it in there you then suppress the part in the assembly or delete it. The new surface will stay as it is and regen fine but on your global ref view you will see that there will be some references missing.


I've made a wee video to help you out here and uploaded it on to youtube, someone else started doing this and I thought it was a really nice way of helping people without actually giving them the part modelled, until we get a video section in here that is... ... admin are you listening??!!


http://www.youtube.com/watch?v=JGUp2G3Kc-w


Paddy

This is a dangerous thing to do as any changes will not be updated into the part with the copied surfaces should any be made. You are best off keeping the assembly which the surfaces were copied into if you ARE going to do this. The other option is the master model merge technique. If you don't have AAX: I have two files: one is original.prt and the other is merge.prt. Merge.prt references original.prt so all the simply need to so is open up YOUR part, rename it temporarily to original.prt, then open up merge.prt, regenerate, then open up your original part in session, rename it and then rename the merged part to whatever you want it to be. Save everything down.
Edited by: pjw