I often use a construction line to mirror entities in a sketch instead of creating one feature and then mirroring it about a plane. Everything seems to work fine until I try to do that with a slot. I can have a fully defined sketched slot but I get an assortment of errors when I mirror it. Am I doing something wrong? I am enclosing a simple part to show what happens.
Thanks for looking,
Glenn
Glen,
Is this using the sketch slot tool or drawing 2 circles with 2 tangent lines
and trimming slot? or both ways.
I would think as buggy as the first one may be because of the constraints that
come along for the ride might cause it to not mirror, but I would think the second
way (hand doing it) would work.
It was done using the sketch slot tool. Deepak's post is interesting showing that there is no problem if the radius is dimensioned instead of the parallel lines.
One would have to ask, why would that make a difference?
But sometimes we have to do what works instead of what makes sense.
Dimensioning to the sides adds an implied parallel constraint that may be considered over defining depending on what other relationships the slot tool, or mirror, has added automatically. I've seen this happen in other situations too.
EriK I may have to disagree as adding side dimension on the mirrored slot works (check the picture in my post above)
Deepak,
I saw your pic' and did notice that there were no obvious errors with either method. I'm on the Mac right now and so haven't looked at the SW part, but I gathered from Glenn's response that he had encountered problems when dimensioning the parallel lines, but not the radius, even though your sketch looks OK. I have seen problems in the past with SW not wanting to allow some relation/dimension combinations. E.g. distance dimension between 2 parallel lines causes over-definition if both lines are picked, problem is solved by picking one or both endpoints instead. This seems to be much less of a problem in recent years (along with similar sorts of assembly mate issues too).
Glenn,
Mirroring sketches is, often desirable to mirroring features, but occasionally peculiar things happen when you mirror a sketch. Both over and under defining. If you have a look at "display/delete relations" you can usually find the error without too much difficulty. Think about what relationships SW tools might be automatically adding. Sketch tools are mostly pretty straight forward and don't seem to do a lot of analysis of what you may already have done. Unlike features, which happily give you lots of vague excuses about why they aren't going to work, sketch tools will shoot first, and turn red later. Is your posted part in 2010? If so, I'll have a look next time I'm on the PC (2011 is still in the box waiting a free moment, or two) then maybe I can give you a more exact answer about your particular problem.
Erik,
And Deepak, please feel free to disagree with me whenever you like.
On some of your points I do agree with you that sometimes SW tends to behave strangely and if you do it other way, it works fine. Not sure if it is asking for a break
Another discovery here: If I change the relationship, then also it works fine
Hello Erik,
Yes, the part is SW2010. I really like SW2010 and have found it to be very stable, and my company didn't renew the subscription shortly after SW2011 was released and I was reluctant to go to it since I wouldn't be able to get service packs. I think I will try to go to 2012 when it comes out.
And to clarify, I did dimension the two parallel lines to define the sketch, but that didn't cause any problems until I did the mirror.
Thank you,
Glenn
Glenn,
Just had a look at your part and without doing a lot of investigation, I'm standing by my original contention. When I made your vertical dimension (slot width) driven and added an equivalent dimension either to the arc (as Deepak shows) or to the endpoints there was no problem with the sketch. I think that there are "overlapping" relationships added by the various sketch tools (slot, dimensioning, and mirror), not all of which show up in "display/delete relationships". When these relationships add up enough SolidWorks gets a little grumpy about it for no real good reason.
I might play around with this some more and see if I can figure exactly what is happening. I have some ideas but it will take a bit to try some scenarios and see. I'll post what I find, don't hold your breath.
Erik,
Seems like a bug as not sure if it is intentional. But if I replace the width dimension with radius on left side slot or give width dimension on right side slot, it works fine.