CAD Forum

Hi all,

I have 2 parts I inherited that are a RH and LH versions, the person who created them mirrored them and as such I had to add a set of tapped holes to both.

The one that was modeled originally, I added the 2 tapped holes and they went in no issues and the detail print recognizes that they are tapped holes.

The mirrored part the holes appear without the cosmetic thread, not the end of the world, but when I go to dimension the 2 holes, I only get the tap drill size no info on tap size.

So is there a proper way for tapped holes to be mirrored or is that one of the short comings of doing this?

Regards,
Jim

I've seen the same thing, and haven't found a workaround. In the past, I've added a pilot hole in the parent part, and then mae the threads individually in each part.

Hi again,

Wasn't worried about actual threads more the detail print callout which the only work around I see is to type out the tap and add cosmetic threads to the mirrored part, so it looks correct.

Regards,
Jim

The advantage of doing it at the part level is it can be used for a feature driven pattern, if needed. Either way works.

If the original mirroring operation was done without checking 'Hole wizard data' in the 'Transfer' section of the Insert Part property manager, you will see this behavior.
I don't think there is a way to toggle that option after the fact. However, I never use derived parts so I may be wrong.

I don't need to mirror things very often, but from my experience with Solidworks, the rule is: Never ever ever ever ever use mirror.

Although I have heard in 2023 that they made some advancements. Not sure if those filter through to the hole callout.

hi,

I will have to check the options set as I stated I inherited it and I am usually also never mirror anything as it always finds a way to bite you in the a$$, if you know what I mean, not to mention as soon as you release a mirror part someone wants something unique to one of the 2.

Regards,
Jim

I just discovered that "Corner Relief" in sheet metal does not carry over on a mirrored part correctly either. The formed part looked correct but as soon as I flattened it the relief disappeared. Our VAR told me the only fix was to add the Corner Relief into the tree of the mirrored part.

DLZ_SWX_User wrote: ↑Fri May 05, 2023 12:13 pm I just discovered that "Corner Relief" in sheet metal does not carry over on a mirrored part correctly either. The formed part looked correct but as soon as I flattened it the relief disappeared. Our VAR told me the only fix was to add the Corner Relief into the tree of the mirrored part.

I did a quick test and don't see that behavior. The corner relief is still there in the flattened mirrored part.

DanPihlaja wrote: ↑Fri May 05, 2023 9:56 am I don't need to mirror things very often, but from my experience with Solidworks, the rule is: Never ever ever ever ever use mirror.

Although I have heard in 2023 that they made some advancements. Not sure if those filter through to the hole callout.

I use the mirror function occasionally, and don't have any issues with it. It's like configurations, which some people also avoid. You need to learn how they work (and don't work).