×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Relations between bodies
2

Relations between bodies

Relations between bodies

(OP)
If I have a Body seperate from my main part (body), is there any way to unite them with relations?  Or add relations before or after the Unite?

RE: Relations between bodies

What version of Nx are you on?
By relations do you mean "retaining parameters"?

RE: Relations between bodies

(OP)
version 7.5.

I'm thinking relations similar to other design features, like when you locate a hole or a boss.

RE: Relations between bodies

Can you provide at least a picture of 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
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

Are these components in as assembly or bodies in a single part file?

If they are bodies in single part file try using...

Edit -> Move Object...

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

(OP)
They are bodies in a single part.

But how can I add any relations with Move Object?

RE: Relations between bodies

In the attached file I created two primitive solids spaced a distance apart. I added a sketch to the cube to indicate where I wanted the cylinder to be located, then using Insert>Synchronous Modeling>Move Face I selected all the faces of the cylinder and used "Point to Point" (center of cylinder face to sketch point)to locate the cylinder.  If the sketch is updated, the cylinder moves accordingly.  This will work if you are not attempting to change the orientation of the solid being moved.

Maybe a more complex set of guide sketched could also handle orientation changes.



 

RE: Relations between bodies

You could also try using Synchronous Modeling, as I did in the attached example file similar to what I suspect you're trying to do.

To see what I've done, just toggled ON (select the box next to the feature in the Part Navigator) the last 3 suppressed Synchronous positioning features one at a time.  Note that the 'Amber' body is dumb and that I used a combination of constraints and dimensions to position to 'Amber' body relative to the 'Light Blue' body.  The last two 'features' are dimensions which you can edit to move the 'Amber' body to wherever you wish it to be on that end face.

When crating these sorts of features where you wish to 'move' and entire body, when the function is asking you to pick something like the 'Motion Group' or the 'Faces to Move' be sure that use one of the selection options, like 'Body Faces' or 'Feature Faces', so that ALL of the faces in the body that you're trying to position has been selected so that they move as a single object.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

In the example model the last three features are already enabled.  First suppress them by seleting the boxes in front of the features and then follow my instructions above.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

(OP)
That seems like what I want.  Thank you.

RE: Relations between bodies

you may combine (unite) the bodies in John's model without any problems

RE: Relations between bodies

Yes, but they had to positioned relative to each other first, which is what the original request was asking about.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

can one use Datum coordinate system for this method?

RE: Relations between bodies

Not sure what it is that you're suggesting here.  Please explain.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

I have a solid part say a shaft.  I have done a nice revolve to create a shaft blank.  Now I need to add splines to this shaft.  we have a nice part setup as a template that has all of the expressions setup to enter the spline data and it creates this spline.

Now I go into insert part and insert this template part and change the expression to my spline I need.

Now I have two solid bodies on the screen.  

In I-Deas we could "join" with relations.  So I would make a datum plane on the solid body of the shaft.  Then attach the coordinate system of the imported spline to the datum plane of the shaft.  So when the spline features moved the spline solid body cut would move with the change.

I can not find a way to attach the solid body part coordinate system to a datum feature on the shaft solid body and keep it associative.  We like to use coordinate and refernce geometry to attach dimensions to.   

RE: Relations between bodies

After inporting the spline, have you looked at using the 'CSYS to CSYS' method in the 'Move Object' command to orient it with the shaft, as described in your example?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Relations between bodies

Reply to Sdeters question:
 I have had a very similar discussion with another I-deas->NX using company, and the approach in NX is slightly different but i hope as good in the end. If you model everything of your spline setup part around a Datum csys, you can then either copy all features but the D-cys into the receiving part, or define a user defined feature that again contains everything but the datum csys. Then when "importing / pasting" NX will only prompt for a datum csys. Done.
  Johns method will produce a "move feature" but should apart from that produce an equal result.

RE: Relations between bodies

John Your suggestion worked BUT.

The Wireframe Sketch did not move with it.  When I click associative I can not have the parents on.  So My wireframe stayed then the solid body moved.  For what I am trying to accomplish this will work.

Toost
When we tried copying pasting I lost all of our Expressions that defines the spline. I have another post on here about that. So we went to file import part that works well.  I think we need to have a coordinate system for our Law curves to come out correctly?  Also On Part import is there a way to have associativity when I select the coordinate system.  I do not see this as an option but there is many options in NX.  I will have to look into user defined feature.

Thanks again both of these posts helped out a lot.   

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources