Hello People, first off -- I'm German and I'm using the German version of Solidworks so I have a profound lack of the proper English technical vocabulary, but please bear with me. I'm designing a part which is basically a square slab with almost identical features on all four narrow faces. The features all have the same shape but are milled out to different depths (which is why I can't use a circular pattern). So I made one sketch on one face first and then put derived sketches on the other three faces. Unfortunately I found that all of these sketches are a mirror image of the original one so all the derived features would come out as mirrored versions. Why is this, and how can the orientation be changed? As far as I can tell, derived sketches can be translated and rotated within the plane on which they were place, but I haven't found a way to flip them. Thanks for any tips, --Daniel
On 12 Nov 2004 09:48:57 GMT, in Msg. <-hamburg.de> ....to be more precise, I've posted an image here: http://www.stoptrick.com/stuff/SWproblem.png On face A is the original feature, which is supposed to be repeated on faces B thru D in different depths. Note that on face D the orientation is correct, but I managed this only by first placing a derivative sketch on face B (where it appeared flipped) and then re-defining the sketch plane (?) to be face D. Likewise I got the feature onto plane B: First plonk it onto D, then make B the sketch plane. However, I'm still stuck with face C: However I define and re-define the plane of the derived sketch it ends up in the wrong orientation once it gets to plane C. Mirroring the finished feature is not an option because it always creates a new copy of the feature instead of just mirroring it. Thanks, --Daniel
Don't apologize for your English. You have better grammar than 90% of the people who post here. It sounds to me like the sketch got flipped on the way to the new sketch plane. There are two possible solutions. 1. Do an edit sketch plane on one of the errant sketches. Change it to a plane 90 degrees from where it is now and then do it again placing the sketch back on the same plane it started from. I have a suspicion that when you used that sketch for a cut it considered the face normal to be pointing inwards while when you derived the sketch to the other faces it considered the face normal to be pointing outward. Moving the sketch from face to face tends to rotate the assumed face normal used by the sketch. 2. Use the modify sketch tool and flip or mirror the sketch if you can.
On Fri, 12 Nov 2004 08:33:24 -0500, Yup, that did the trick. In my picture at http://www.stoptrick.com/stuff/SWproblem.png I moved the sketch A->B->D->C and it came out right. Weird! There should be a way to define the face normal for a sketch. Thanks a lot, --Daniel
Yes! This is a really basic function that SW doesn't want us to have, for some perverse reason. And, as Paul said, you have no need to apologize for your English. Remember the scene in "My Fair Lady" where the Hungarian linguist "proves" that Eliza can't be English because she speaks English too perfectly? That's how we know you're not a native English speaker. Jerry Steiger Tripod Data Systems "take the garbage out, dear"
You can use a circular pattern with some creative thinking. This is why there is the option to do a geometry pattern and not. Try this 1) make your square block. (You are done with this) 2) draw on the large face of the block a rectangular sketch representing each side would represent the depth of the cut you want on that side. 3) extrude a surface body out of your new sketch. 4) create your first profile sketch. 5) extrude the profile sketch (use "up to body" and select the surface body you made in step3 6) circular pattern make sure the Geometry Pattern option is OFF. and there you have it. A different depth for each cut. you see since your extrude cut was "Up to body" it recalculates what this means for each instance in the pattern. regards, Corey
On Fri, 12 Nov 2004 13:12:39 -0800, I'm beginning to feel like a stupid idiot trying to fish for compliments. But I'm not! All I wanted to say was that I neither know the correct English terms in technical construction, nor the English menu entries of Solidworks which might make communication in this group difficult (because it's hard to "walk" someone "through" a software where everything is labelled differently). As it turned out, my language concerns were unwarranted. Thanks for all your help. I did manage to work around this problem myself (like described), but I'm satisfied to see that this is really a lack of SW's functionality (an odd form of satisfaction, given that this is a deficiency of a piece of software I regularly use). Thanks, **Daniel
On Fri, 12 Nov 2004 16:16:08 -0600, in Msg. <> [good hints] Clever! Did it differently, but filed your suggestion for future reference. --Daniel
