yup, that's also a solution. Downside: it's a part copy
in both cases without any history.
When you have a need for the two parts then with the first
solution (mirror copy) you have this option:
after mirroring the part you can then split the part
by using the 'Divide Function' which will create
2 parts which are related to one, the 'Master Part'
Going off at a slight tangent here - I would avoid creating opposite hand parts with the insert part cop/mirror command unless you are absolutely certain that you will always require both parts.
For example - I'm working on a job at the moment where someone has created the mirrored version of a machine and some of the parts are mirrored part coppies. Unfortunately only the mirrored version is used in the machine (and only the mirrored version is drawn !), so when I come to modify the part I have to go back to it's original and modify that one -- GRRRRRRR!!!
Depending on how complex the part is, you could use the direct edit tools to make modifications of the part copy and leave the original as is. I've even started experimenting with using copies of an original part then stretching, adding holes and other featuers using direct edit to make longer parts etc. This seems to be a simpler approach than using families of parts.
Hi Kyle,
Yes you're quite correct, and these are valid and extremely useful methods when applied correctly. It's just that in this case the original part was copied for the new project but was NEVER going to be used. Only the mirrored part is used.
Again going off the point slightly here, this particular customer creates an entirely new set of models and drawings for every project - and that's about 1000 drawings - even if they are identical to previous projects. Hard to believe really - but it's great for us contractors !!
I just tried a mirrored part copy and SE won't let you break the link. I think the only solution is to use the mirrored part copy and maintain the link or export the mirrored part copy as a .sat, STEP, parasolid etc. Of course, now you have no history on the part.
On your second comment, do you use Rev manager to copy the drawings and models to save time. I did that when I made a new revision to drawings that also now needed to be linked to family of parts members and it worked perfectly.
you can break the link. Once your part is copied, open or edit the mirrored part. Modify the part copy feature. Click on the change settings/parameters button in the SmartStep ribbon bar, and in the dialog box that opens, uncheck "link to file".
I have no idea why you can't do that while you're creating the part...
BTW my terms may not be all correct as I'm working on a French version...
