I have a part that was given to me with the part being not in line-of-draw. The part is all contoured (no flat planar surfaces). I was able to create reference planes on the part to get a plane eventually that represented line-of-draw. How can I align the part to the main plane using this reference plane? I know I can create the tooling split without doing this step, but, to make things easier down the road, I prefer to have the part aligned to the main part coordinate system.
Jeff,
You should be able to use ethe Move / Copy bodies to move & rotate your part.
Thanks,
Andy
Thanks Andy. But the problem with the move/copy bodies command is that it will not allow me to mate the created reference plane to the main front plane. It says that I need to pick a different entity from the moving body.
Jeff,
Without knowing exactly how you created the reference planes I'm guessing that your problem here is that the plane is defined by the part and so you can't use it to then realign the part. One of those circular reference things.
You may be able to use Move/Copy... if you can use the same features you used to create the reference planes to locate the part on your main (Top?) plane. You may have to Move/Copy.. more than once to get it completely realigned.
You don't say your part is imported so I'm assuming it's a native Solidworks part and you would prefer to retain editability.
If you are dealing with an imported "dumb" solid, Doug's method is as good as any, you don't lose anything by exporting and reimporting the part.
Another way around this problem is to put the part in an assembly using the plane you created to position it. This adds another assembly level but if that's not a problem for you it's a relatively simple way to move the part.
If you can post the part it's possible someone can make a better suggestion. Click on "Use advanced editor" in the upper left corner to attach a file.
Jeff,
Have you tried inserting your part into a new part, then use the move / copy bodies to locate?
Thanks,
Andy
Position the part the way you want, then hit your space bar and choose the icon for "Update Standard Views".
This will do nothing to alter the parts orientation in relation to the origin.
Create an "L" shaped sketch on the reference plane you created...with the two lines pointing in the directions that you will want the "X" and "Y" origin axis to be...and exit the sketch. Then create a Coordinate System using the intersection of the two lines as the "Origin" and the two lines being used to define the "X" and "Y" direction. Save as, Save as type = Parasolid (*.X_T), Options, Output coordinate system...select the one you just created from the pull-down, OK, Save.
Open the parasolid file. If you did it right, it will come in oriented how you want it to be.
1)Click on the main plane that you create, press spacer bar, select normal to.
2)Click on standard plane that you want to be (Front,Back,Right,Top or Bottom),then press update standard view.
This will do nothing to alter the parts orientation in relation to the origin.
Since you say the part was given to you, I'm guessing it is a dumb solid. If that is the case, why not insert your part into an assembly, mate the part to the origin and planes as you want it and then save it as a part?
Thanks all for the suggestions. Since it is a "dumb" solid, Doug's response makes the best answer for me. I thought about making an assembly of the part and mating it that way. That would probably be okay too. I will have to mess around some more with the "updating standard view" idea. I still was never able to get this to work out correctly.
Create an "L" shaped sketch on the reference plane you created...with the two lines pointing in the directions that you will want the "X" and "Y" origin axis to be...and exit the sketch. Then create a Coordinate System using the intersection of the two lines as the "Origin" and the two lines being used to define the "X" and "Y" direction. Save as, Save as type = Parasolid (*.X_T), Options, Output coordinate system...select the one you just created from the pull-down, OK, Save.
Open the parasolid file. If you did it right, it will come in oriented how you want it to be.