Modify the diameter of a dumb model

[Trietsch]

Hello,

I am trying to modify the diameter of an imported model with no history. It is a simple cylinder with chamfers on the four corners. Each time I try various options in synchronous modeling the options to keep the cross section constant end with a failure. I can get the OD or the ID to move within limit of the chamfer, however I can’t seem to get both the OD and the ID along with the chamfers to move together. I think this is what the coaxial option in face finder is supposed to do, however it ends in an “Invalid face or face type” error.

Any thoughts would be greatly appreciated.
NX 6.0.5.3
Thanks,
Ryan

 

[cowski]

Delete the chamfers, offset the faces, reapply the chamfers.

In later versions (NX 7.5 I think) there is a "label chamfer" command which would probably do what you need, but I don't think it is available in NX 6.

www.nxjournaling.com

 

[Toost]

Check the face type of the presumed cylindrical faces. Information - Object - select the face and read the geometry type.
Since it's imported it might be more complex than expected. ( In NX it would have been "cylindrical" or "extruded")
You can try run the part thru the File - Export- Heal Geometry and try again on the "healed" model. ( It will create a new partfile.)


Regards,
Tomas

 

[JurgenKreisel]

In synchronous modeling there is an "optimize face" option.
This has helped me in the past.

NX 7.5

 

[JohnRBaker]

Can you provide either the model itself or at least a picture of what it is that you're working with and what it is that you're attempting to do?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cowski]

In synchronous modeling there is an "optimize face" option.

Not available in NX 6, another goodie to look forward to when you upgrade!

www.nxjournaling.com

 

[Xwheelguy]

Something this simple, is remodeling out of the question?

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[capnhook]

Yeah......like, when are there four "corners" on a cylinder. A cylinder has three faces and two edges, not four faces and four edges, eh?

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[Xwheelguy]

A cylinder with both an ID and OD indicates to me a hole through it, which would have 4 edges, no? But I do see your point, just have to sometimes read more into what people are trying to say, but images always are the best help, IMO.

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[Trietsch]

Thanks for the help, in this case yes it would be very simple to remodel the part, however this is a common problem that my colleagues face from external CAD services like the link below (you'll need to create an account if you want to use it). My particular example was imported by a colleague so am not sure the origin, nor translation process, which could be part of the problem. Also it was scarf (or angle) cut which I could use the replace face command to remove, however the cylindrical surfaces were split into 3 faces each. It was part number GP2C19000 if anyone wants to try a parasolid or other format.

http://www.tss.trelleborg.com/us/en/service/cadservice/cadservice.html

You can get a file for fractional sized parts, I'll attach a 6" piston step seal. However, I may need a 6.050" sized part, or anything off of what the CAD service can provide. It would be nice to be able to use this technology to modify the diameter and keep the cross section constant, without needing to extract cross sectional curves, and revolving them at the new diameter.

We are also using TC 8 JRE 1.6.0_14 once the file is translated if that is of any interest.

Thanks,
Ryan

 

[cowski]

I used the join face command to merge the faces, then label chamfer, and finally offset region. Faces updated no problem (using NX 8).

NX 6 does not have label chamfer, so you may have to delete them and reapply them after the offset, or perhaps use the edit cross section command to get what you want.

www.nxjournaling.com