Just looking for suggestion on how people handle handed parts.
We do mostly cabinet panels.
2 ways I’ve seen it done here. Both Configurations of a single part.
Mirror Body/Delete Body as the last step.
To modify you roll the tree back before the mirror, do your modification and roll to end.
2 extra steps in the tree but very manageable.
2.“Edit Sketch Plane” configuration specific.
To modify you edit the sketch plane, select the new surface, specify, “This Configuration” and your done.
Personally I like the Mirror Body/Delete Body (wish it were 1 step). Simple and straight forward.
The Edit Sketch Plane I like because it’s a single step but I worry that a newbie would be confused by this method. It’s buried in the feature ad most people wouldn’t know how to find it.
I do not like “make handed part” at the assembly level. The external link (again) would confuse a newbie.
I was wondering how others make handed parts?
looking for opinions.
Option 1, with two configurations. One configuration with the Delete Body feature suppressed and the other with the Mirror body feature suppressed. (Maybe that’s what you’re already doing, but you didn’t go into that much detail.)
We’ve been doing mirrored parts as a copied part that references back to the first file for years. Although that was Solid Edge, the method has been working in Solidworks so far. I’m curious why the external reference from a left hand file to the right hand file (or visa-versa) is not an option.
Having more that one part number in a file is not an option here. Well, a very bad option at best.
I’ll agree that not making them with a Mirror component feature in an Assembly probably isn’t the best solution, but for people who don’t want two Parts in one file then pre-selecting a plane in the Part and going to Insert > Mirror Part… is a pretty good option (if you don’t pre-select a plane it will be grayed out).
I don’t like this idea because it’s basically a ‘insert part’ with a fixed mirror plane. Correct me if I’m wrong, please!
I think using insert part & then mirror around a plane of your choosing is the more flexible way of doing it.
I found ‘Keep Body’ to be the more stable version. For whatever reason some parts kept having a feature error regularly when we deleted the bodies instead of keeping them.
Edit:
If you’re doing configurations, I think option 1 would also give you a little flexibility:
If the other handed version has a SLIGHT difference It’s easier to see if you place the differences(aka new features) after the mirror & delete/keep body features.
Also if you work with sheet metal option 2 does not really work with bends.
I’ll agree wholeheartedly with this one. It just works..
And I handle filenames in the configuration too.. Simply the same filename (Using code [$PRP:“SW-File Name”] suffixed with .L-or-.R
Again, agreed.. And the way assemblies handle opposite hand parts is stupid. A mirror is a mirror… Not a variation of some form of pattern..
Tho, I believe there is an option to enable mirroring the part within the part and not create a separate file..
. . . and the way the Mirror Components feature handles non-opposite hand parts is often stupid also. Too often they’re placed like it was a circular pattern instead of mirror.
Also doesn’t work if using PDM and serial number generator for filenames. The PDM Addin missed the SW events that create a new file without using the Save File Dialog, so getting a serial number file name for these parts takes several extra steps that should really be done when none of the files are open.
It seems there’s a consensus that using the mirror part in assembly environment is least desirable if not always bad.
