Creating a reconfigurable assembly in NX2 2

[mhf23]

Hi,
I'm modelling a bit of tooling in UG NX2 at the moment which has two separate modes: put the components together one way it does one job, put them together another and it does a different one. It's really too simple to use subassemblies.

My question is this: is there some way of configuring one assembly model so I can have only one instance of the component and easily swap between the two configurations? NX help suggests reference sets (not keen - as I understand it this will mean only one configuration is properly mated, and the individual components end up modelled twice) or variant configuration (the help file tells me how to edit one but not how to create it!). Anyone able to point me in the right direction? Thanks!

 

[feadude]

you might want to try:
Assemblies
component
deform part

 

[mhf23]

Thanks dude, but this isn't like a spring or a clamp which fits together in two different positions. What I'm aiming for is more like... two table tops fixed together, with the ability to flick between having the table legs attached to one table top and the other - without having twice the number of table legs in the parts list. Can deform part do this?

 

[feadude]

Define Deformable Part
The Define Deformable Part dialog lets you designate a component as deformable and define the shapes into which it can be deformed.

You must be in the Modeling application to use this dialog. It is available at Tools-> Define Deformable Part.

To allow repositioning of a deformation in coordinate systems other than the absolute coordinate system, you must ensure that you provide sufficient references and direction expressions. For example, we recommend that you create extrusions by extruding a sketch instead of simple part curves, because the defining reference plane can be included only with a sketch. Also, be sure to include expressions that control directions, such as offsets on an extrusion; otherwise, you will not be able to readjust them if they are incorrect in the destination coordination system.

The Define Deformable Part dialog has five pages: Definition, Features, Expressions, References, and Summary. To open a dialog page, click on the box beside its name in the left column.

Common Items
To move to another page, in the left column of the Define Deformable Part dialog, select the box beside the page that you want. Or you can use the Back and Next buttons in the bottom right corner of the dialog.

The images at the top of the dialog, as well as the boxes in its left column, indicate the page of the dialog.

 

[PennKoff]

hi Yucc

have you tried arrangements?

you can define arrangements, then define arrangement specific mating conditions

_____________________________________
"...standards are great because they give nonconformists something to not conform to..."
_________________
Penkov, Peter I.
Non-standard Equipment Designer

 

[PennKoff]

moreover

you can edit suppression state and some component can be present in one arrangement while in another that component can be suppressed

_____________________________________
"...standards are great because they give nonconformists something to not conform to..."
_________________
Penkov, Peter I.
Non-standard Equipment Designer

 

[mhf23]

Thanks Pennkoff, that sounds much more promising! One minor problem, though - I'm actually running NX not NX2 (my bad, sorry) and I can't find reference to this command. Is it something specific to later versions?

 

[PennKoff]

hi

it's a good question. (-:

i think you need nx2 or nx3 for arrangements. sorry i'm not helpful. may be someone more experienced in the business will help you.

success

_____________________________________
"...standards are great because they give nonconformists something to not conform to..."
_________________
Penkov, Peter I.
Non-standard Equipment Designer

 

[motorsportsdesign]

You can suppress components by expression in NX, that is a very easy way to do it.

Jonathan T. Schmidt

http://www.schmidtmotorworks.com

 

[cloche]

suppress by expression: very nice, I didn't know it! Do you mean that 0=suppressed and 1=unsuppressed? And how must the variable be called? How do you "link" it to the status of the component? Sorry for these questions that may sound stupid, but I'm somewhat new to UG and moreover for the moment I only dealt with single parts...

 

[mhf23]

Thanks [motorsports], but I'm working with UG in iMan (or Teamcenter as it is now), and if I simply suppress components they'll still turn up in the bill of materials, won't they? I don't want to end up ordering twice as many bits as I need...


Matt Freeman,
Design Engineer,
UK

 

[dks123]

I run into this problem alot. Here's how I deal. While in the assembly I use Wave Linker to produce a new non asociative body from each component I need to show relocated. When I have all the bodies I need, (they will still be linked, as evidenced in the model navigator) I then "un"link them by using extract body. Finally I used tranfer copy delta 0,0,0, on all of the extracted bodies. This will create uanprameritized bodies in the model navigator. I then delete the linked and extracted bodies from the model navigator leaving the unparamaritized bodies. I then put these unparameratized bodies in a diffent reference set. It is really not as laborious as it sounds an

 

[dks123]

If mating conditions are important to you try using exloded views.

 

[Kirsten]

Here's a way (in NX2, at least) to keep parts from showing in a parts list. In your drawing file, highlight the part in the ANT that you don't want to show in the parts list. Then right-click, Properties, select the Attributes tab, and in the Title field enter
PLIST_IGNORE_MEMBER
or
PLIST_IGNORE_SUBASSEMBY
depending on whether or not it's a component or sub-assy.

In the Value field, enter anything you want (I put in "Hidden"). I wish I'd known about this long ago.

 

[feadude]

If you just do not want to see it in the parts list, I think you can just delete that row.

good57morning@netzero.com