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.
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
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
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.
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
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.
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.
