Assemblys and material removal

[fighterpilot]

I have an assembly of two parts. Each part is a separate UG file. I created a new assembly and assembled the parts together (mate, align, etc). Now, to mimic reality, I need to machine a feature in one of the parts. I sketched an outline of my machined feature and then created an extrusion I hoped I could subtract from the part. No go. The option to subtract is not even there.

Question: Is this type of activity not possible in NX5? I assume I'm missing something because other CAD systems have been doing this sort of thing for years.

If not possible, how to I need to approach this sort of design?

Thanks...



--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

You can either use promotions or wave-link, and subtract from the resulting part.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[fighterpilot]

I think I found what I needed. Insert/Combine Bodies/ Assembly Cut.



--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

For what you're trying to do I would model you 'tool' body as you've already done (in the context of the Assembly I assume) and then use:

Insert -> Combine Bodies -> Assembly Cut...

It works just like a Boolean Subtract and you don't need to WAVE link or move objects from file to file.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

Now I wish to "pattern" this feature. Associative Copy in UG terms I believe. I'm not able to select the assy feature or the sketch used to make this feature.

Any help appreciated. Pro/E experience is hindering ability to use UG. May just give up.

Thanks..

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

I'm obviously stuck pre-NX5...

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Create your 'tool body' as a solid but don't use the Assembly Cut function quite yet. Now use...

Insert -> Associative Copy -> Instance Geometry...

...to make your 'array' and then perform the Assembly Cut operation selecting the multiple tool bodies in your second pick.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

OK. I understand now. Now I wish to insert a hole feature but intersect the two parts. It's only letting me pick one part to put my hole thru. Do I not use the hole feature but use the assy cut feature?

Patience appreciated.

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

Try using a 'Hole Series', which was added in NX 5.0.3.x. If that doesn't work, set the Boolean in Hole to 'None'. Now you have a body that can be used like any other solid body in a Boolean/Assembly Cut operation.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[NXMold]

In ProE I did everything in the context of an assembly, you were absolutely unlimited in making interpart references anywhere and everywhere as if everything was all in one place (as it appears on the screen!).

Not so in UG, where you are working wholly in separate files, that only have a faint appearance of being assembled or related. Try to keep that in mind, and consider that whatever you do it should be possible without being in the assembly.

If you have a complex shaped flange in a base, and need to model a matching flange in a cover, you cant jump into the cover and start making extrudes. You have to wave link a composite curve of the flange profile, or link a face, etc. Then you have enough data in the cover file to start modeling.

When placing a hole thru two parts, if it is for a screw or pin you can model the "false body" in the pin. Perhaps extract the body and offset the diameter for clearance using direct modeling, then link that body into each component and subtract it. I havent had a chance to use the new 'hole series' feature yet, but have created holes in the first part with the boolean set to none, then that body into the second part before subtracting it from both.

NX 5.0.3.2 MoldWizard

 

[fighterpilot]

NXMold,

I've been having a difficult time moving over to UG. I moved to CATIA V5 with ease but I just cannot figure out what UG is looking for sometimes. I've asked people here about how to do certain things in UG as I did in Pro/E and I get the "glassy eyed" look most of the time. I told them about Pro/E's ability to "show" dimensions when doing a drawing and you'd swear I was speaking in a different language.

Someone tried to explain to me what I needed to do in the assy to make machined cuts and I ended up glassy eyed. The NX "Product Evangelist" in this forum has helped me understand but it still seems way more difficult than the way Pro/E approached the issue. I didn't have to think of boolean operations in Pro/E as it was all handled in the background.

Hopefully this won't start a Pro/E v. UG discussion but I'm just trying to understand some of the underlying ways UG does things.

--
Fighter Pilot
Manufacturing Engineer

 

[ewh]

That is a downside to NX, though the reasoning for it is good. Legacy modeling methods are maintained, so every time a new method is implemented, the software gets that much more complex. This leads to many different, valid ways of accomplishing the same thing.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Note that in NX 6 we have implemented many more modeling functions which will be allowed in the context of an assembly that will NOT require the user to perform explicit WAVE links nor to move constantly from one file to another.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[NXMold]

I love working in UG, its so much more flexible than proe was. You have to find ways to take advantage of that though, because while it has many of the abilities of proe, they are... less mainstream, and not as well implemented.

NX has its roots in legacy non-parametric modeling, leveraging that can be a real boost in productivity.

For example, in a mold design when a customer sends a changed part model it must be added to the assembly. Its coordinate system is way out in space someplace, and the part may not have good geometry or datums to make assembly constraints (mate, etc). You can assemble the new model inside the old part model using the absolute csys, then go back to the top assembly and drag the new model out to wherever you want it in the assembly tree, and delete the old model. It keeps its position/orientation. No need to reposition, move, or constrain it.

Sketch profiles/section curves, extruded bodies, and boolean operations are all (mostly) separate where proe combined them in a single step. I like this way, as I create VERY few sketches anymore. I do a lot of simple lines, say from midpoint 1" along the Y axis, then extrude that.

If you have any specific questions or examples I can try to elaborate more.

NX 5.0.3.2 MoldWizard

 

[DavidTolsma]

John, can you explain why you would not want to create a Geometry link to the machining file? I'm not familiar with Assembly Cut, can I then share the machined Assembly Cut file into assemblies, CAM files, Drawings, etc?

-Dave Tolsma
Tolsnet LLC

http://groups.google.com/group/NX_CAX/

http://groups.google.com/group/plm-exchange/

 

[JohnRBaker]

Yes, the resulting assembly, with the Assembly Cut features in it, is like any other assembly file which can be the master for any downstream manufacturing, drawing, etc, file that you wish.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[fighterpilot]

John,

Can you explain why I just cannot "show" dimensions of my features in a drawing ala Pro/Engineer? Am I missing something?

Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

If you created everything in NX using fully dimensioned/constrained sketches, as is the norm with Pro/E, then you too could just 'Show the Dimensions' when you make a drawing.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.