Mirroring a part

I modeled an existing part and now I have to model another part that is
almost identical, except it's the other hand. I did a Save As to the first
part and now I need to mirror it and switch the location of a couple holes
and add some other features. When I try to mirror the part (Insert, Mirror
Part...), it creates a whole new part in a different drawing. That's not
what I want. When I try to mirror the part (Insert, Pattern/Mirror,
Mirror...) it mirrors itself without the option of deleting the original
part. That's not what I want, either.

Is there any way to mirror a part without having a copy of itself? What if
a guy has a few days design time into a part just to find out that he needed
the other hand? Does he have to start all over?

Relz

 

If you pre-select a plane to mirror about and then go to TOOLS/MIRROR
PART you will create an exact opposite hand copy of the original part
in it's own file. The parts are still linked however, if you change
the original the mirrored version will update accordingly. Changes to
the mirrored part will not propogate back to the original.

 

Relz,

Do Insert\"Pattern/Mirror"\Mirror method. Then in the "Bodies to
Mirror" portion choose your body (skip the Features and Faces to
Mirror). Then under the Options portion, UNCHECK the "Merge Solids"
choice. Now click O.K. You should end up with 2 bodies in the part file
(the original and the mirrored), you will then have to Delete the first
body.

Is that what you want?

Ken

 

It's what I want except when I delete the first body it deletes the mirrored
part with it.

Relz

 

Use The Icon "Delete solid/suface body" it looks like a box with a "x" on
it.

Mike

 

This is interesting. I just tried a few things and, while not perfect as
you maybe would like to see, it's not bad. I created a simple part with a
total of 3 features, and then decided I would actually like a mirror of it.
So, Insert \ Pattern/Mirror \ Mirror, pick the body to mirror, and do not
merge the two solid bodies. Then, as stated, do a RMB on the original body,
and choose Delete body.

This does, in fact, make the body disappear, but its structure of features
is still there. You can then continue building on the mirrored version by
adding holes, etc. If you want to modify one of the features before the
mirror, you can't just double-click on the model, you have to do your
clicking in the FeatureTree. Makes sense when you think about it -
attempting to double-click on a model that is not the "direct" result of the
feature. (Could be an enhancement, though.) Notice that when you modify a
sketch dimension, the sketch appears in relation to the original body, not
the mirrored one.

You will also see that if you roll back above the body-delete feature, the
original "reappears." So, the obvious observation here is that the geometry
of the original part is still intact and can be modified directly by rolling
back.

WT

 

I talked to a guy this morning from a Solidworks school and he didn't have
the answer either. He contacted Solidworks directly and they told him that
this is the most requested missing feature by Solidworks' customers. He
said that Solidworks is working on getting this feature into the next
release.

I'm the guy at our work who has been put in charge of figuring out if our
company should go with Solidworks or another modeling program. I've started
into a project and this is the only speedbump I've come across so far.
Since our company relies heavily on mirrored parts and mirrored machines,
I'm not sure I can fully recommend Solidworks. I may have to look more
heavily into Inventor and see how they compare. Any comments?

Relz

 

Just as an after thought, be careful, if you wish to use the part and
mirrored part in mirrored aseemblies.
When adding changes to either part, ensure that you have EVERY file open,
that are referenced.

 

After doing the mirror, select the body from within the "Solid Bodies"
folder at the top of the Feature Tree. There should be 2 bodies in
there and you should delete the 1st one. Works fine here.

Ken

 

This did work. My only concern now is that it seems to have lost some of
its features, such as a pop-up description of a feature when you hover your
cursor over it. Also, it seems to have lost the ability to highlight the
feature when clicked on in the Feature Tree.

I can get along with your way of doing it, Ken. Thanks a lot and I'll wait
for the next release to see if Solidworks has changed anything.

Relz

 

Relz,

Sounds about right, and don't hold your breath ;^)

Ken