placement of part created in assembly work space

[pc-6]

I have created a new part in a assembly work space.
How do I move the part? It has no constraints applied to it and I am unable to shift its position.

Thanks
Leif

 

[DavidJ]

Precise placement tool.

Shift key + drag for free rotate.

Apply constraints.

Click and drag the part.

All these assume that you have come out of part editing mode and are back in assembly mode.

 

[Max]

By default the first new part you make in an assembly workspace is automatically anchored. If you are unable to move your first part, this is probably the reason. Right click the part in 3D or find it in the Design Explorer and uncheck Anchor.

Max

 

[pc-6]

This is the first part that was made in the assembly workspace. It is not anchored. I have also gone in and edited it and taken out all the constraints. When the part was originally made I used existing lines from other parts as a reference to create the part. With all this done the part still does not move.

 

[DavidJ]

If 'project to sketch' was used with 'maintain associativity' then you effectively have constraints built in. Since you say this is the first part in assembly, I presume it was originally built in another assembly??

Could you explain a little more?, it sounds like we don't yet have the full story, or we are misunderstanding what you have said.

 

[pc-6]

Had some help via PM
So to clarify for others interested and to David J, I had to go into interdesign relations and delete all the associated relations. Once this was done everything was free to move.

Thanks Max and David J for your input.

 

[DavidJ]

Yes - that's what happens when you use project to sketch with 'maintain associativity' between parts, it creates an interdesign relationship.

If you don't select 'mainatin associativity' it is a one off snapshot, so there is no restriction on movement.

 

[Max]

Just for reference, there are a few other ways to create interdesign relationships without projecting sketches, for example by sketching on a planar face of an existing part. In this case, the sketch definition (what plane it's on) references the other part as well and is also an interdesign relationship.

 

[DavidJ]

Good point Max !