Problems in NX8.5

[Gokulkrishna]

Hi,

I have been facing 3 problems while modeling in NX8.5

1. Lets consider I'm making a cube with the length, breadth and heigth and then controling them from the part families table. Now the issue is like if i edit these parameters from part families spreadsheet they get updated in the model but the vise versa is not possible i.e. if I edit the dimension in the model or through Tools --> Expression it doesnt get updated in the spreadsheet. I need it to be bi directional, is it possible?
2. When I save a as particular model to another name and by chance it is deleted, then I'm unable to use the same name for another file. NX show an error that this name is already in use even when it was deleted. Is there a way to clear the history in NX.
3. While using NX part families consider that I have "n" number of configurations in a master model. How will I come to know which configuration the master model is in. The person who has created the model may know the config but if a third person open it how will he come to know that.
4. While making a sketch for a revolve command,currently to enter a diameter I have to enter dia/2 expression. Is there way to enter the diameter directly without an expression or externally calculating it like in case of SolidWorks?
5. Is it possible to open the master model from the child/clone and vise versa?

Thnx
Gokulkrishna Goli

 

[Xwheelguy]

If you want to sketch with diameters, mirror the profile about the axis of revolution and make the mirrored profile reference - then dimension to the reference diameters.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[cowski]

5. In the assembly file (assembly navigator) right click on the component and choose "Make Display Part". In the part file (assembly navigator) right click the part name, choose "Display Parent" and a list of parent parts (which are currently loaded) will appear as choices.

This answer is for native NX, if you are using Teamcenter you may have different options/choices (such as looking up a where used report).

www.nxjournaling.com

 

[looslib]

1. The family tables are not bidirectional. The master defining the geometry is the spreadsheet that is used to generate all family members.

2. Log out of NX and restart will clear the memeory of that part file name having been used. You may also check your working directory to see if NX has placed a copy of your file in there temporarily and it is still out there. However, if you are in a PLM system, it has its own rules and procedures.

3. Let's keep terminology correct. Memebers of a family table are not configurations. Configurations is a viewing option to display different aspects of your assembly. When the assembly is loaded, the structure will show which family table member(s) is/are loaded.

4. Pro/E does a diameter dimension in sketcher by selecting the line, the center line, then the line again, then place the dimension in your view.

5. Cowski answer this in his usual fine manner.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

To start with, it's going to get very confusing very quickly for people to respond to 5 totally unrelated questions all in a single thread. In the future, please start a separate thread for EACH inquiry.

As for your multiple questions:

1) Has already been answered; basically Family Table spreadsheets are, by design, one-way. Once created, the Family Table spreadsheet DRIVES the models, not the other way round.

2) Again, it's been answered; during an NX session file names are unique. If you do a Save-As, even if the file gets deleted off disk during the session, NX as taken that name FOR THAT SESSION. You'll need to exit NX and restart your session.

3) I think I understand what you'e saying, and generally speaking, unless you've gotten really creative with how you've populated your spreadsheet, the first Row of the spreadsheet represents the 'configuration' of the Master Model. Now if you do edit that first row so as to no longer match the Master Model and you place it's parameters in some other row, and there's nothing that says that you can't, then that's YOUR responsiblity. And BTW there's no real requirement that ANY row of the spreadsheet needs to correspond to the Master Model. In other words, the Master Model may NOT be represented by ANY of the records in the spreadsheet. Again, there are NO rules, just conventions and it's up to you to set and maintain standards and enforce workflows.

4) While it is true that we don't yet have a true 'Diametral' constraint dimension, you can do something pretty close by simply creating a 'Mirror Curve' about the intended axis of rotation to act a 'reference' for the 'Diameter' dimension (remember to actually set the status of the this curve to be 'Reference' so that it's ignored when you create your revolved body), as shown below:

5) With your Assembly loaded, go to...

Information -> Assemblies -> Family Report

...and you will get a report flagging all of the Family Members in the Assembly and with that information will be a reference to the names of the Master Family part files for each unique Family Member found in the Assembly.

Anyway, I hope this helps answer you multiple questions.

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.