How exactly can I create a part off of another part in an assembly? Im wanting the newly created part to be tied to the existing part of assembly. I have tried looking through the SE tutorials, and the SE book we have at work. Every option is either too vague or for an older version of SE.
I come from Solidworks, and all you have to do is select "create new part" and then you pick a surface of plane to sketch on. Im assuming that SE can function in a similar way?
Thanks for the help.
There are some ways. It depend on what kind of modeling method is used by you.
Here are some videos, if you use traditional (history based) method:
- Top-down design with master sketches
- Top-down design with assembly sketches
-Top-down design with mixed mode
If you use synch mode this will very simple you have to select a command (Extrude) and select a surface on the "partially hidden part"...
I already found that, and I cant get it to work. Every time I go to create my new part, the base part or assembly goes partially hiddened and I cant tie any geometry. Im just assuming that there is a setting or something simple that is keeping it from working.
OK, you're pretty much there.....just start building geometry as you would in a bespoke model, but you can now access/reference key points and faces from the ghosted assembly, by using "inter-part copy" [or directly off a face in Synchronous]....or "include" within a sketch.
Design Manager Streetscape Ltd
Solid Edge ST10 [MP2] Classic [x2 seats]
Windows 10 - Quadro P2000
Solid Edge makes your other parts semi-transparent. They can be completely hidden by using CTRL+Q. It's a toggle, so use it again to show them. When sketching in your part, insure that Peer Edge Locate is turned ON (button labeled "Peers") so you can find the edges of adjacent parts.
I had the same questions getting started. There is only one way to use existing geometry (with out copying a sketch or part), the "include command". This projects a line from another part into the plane you are working on. The other big learning curve step for me was gettin the plane to work on. Assuming you are creating an assembly part in place, the plane must be in the assembly (not from an existing surface or other part's plane) and then it can only be selected with shift held down. This forces you to create duplicate planes in the assembly as a place holder for planes that exist in other parts that you can actually use.
The bid choice when doing this is do you make it associate or not. Associate lines will update with the parts they were projected from.
If any have another way other than "include" I want to know. I was very frustrated getting started that I could not "snap" to visible geometry.
When you are sketching there is a group under the tools menu called "edge locate". This is where you find the button entitled "Peers". Select this to be able to pick edges from other parts besides the one you are working on. Most of the time this drives me crazy so I only select it when I need it.
omg Iking. I have been looking for this since I started using the program. I have been using "include" for the purpose of this. Now I can get at points rather than just edges.
thank you thank you thank you !