Sketch rotation

mating dosen't require a part to be modeled/oriented in any particular fashion. that's the beauty of mating. it can rotate, flip or whatever to get part in correct location/position.

check out derived sketch.

OK UM...

Make a new sketch. Convert entities. Tools>Sketch Tools>Circular step and repeat. Select the converted entities. specify the angle and the centerpoint of rotation Change the converted entities to construction lines now the new entities should be under defined. add an angle reference and you should be able to control the angle reference in the design table

Is this what you wanted?

Corey

i did the same ... although i can't quite tell for sure, it appears i may have read something in between lines that wans't there. :)

Hi again martin,

STOP! Bad logic!!!

I cannot think of a good reason to make the model so complex when mating is easier! The logic should be to:

1 make the part as the part must be in reality. no fudging.... 2 if you have some features that change on the base part, make configurations and hide / suppress as needed 3 make the required mates in the assembly. then make assembly configurations that have different mates (suppress the ones that do not apply in each configuration). Works great!

One of the things that I remember being frustrated with was the concept of configurations and how they relate to assemblies. Always remeber that if you have a part it a subassembly in an main assembly, that you will need configurations in the part (A, B), then in the subassembly (partA,B) and in the main assembly (subAssem A, B).

Hope that helps.

Well, I've been wondering about this too.

My reasoning is that it is less work. The assembly in question will have some sixty of these parts. I am designing the part with smart mates. And so, when placing the part, you choose the configuration (primarily a rotation change) and click away. The part aligns itself and the rotation comes in for free.

The alternative would be to make a part without configurations. Then you'd have to place some sixty of these on the assembly...and then go through each of them, one-by-one and rotate it to various angles. The good news is that it is a z-axis rotation only, not a muliple axis rotation.

I suppose that another idea may be to place one part for each rotation angle, mate and rotate as required, and then copy-drag each part to where specific rotation instances are required. The trouble with this approach (haven't tried it) is that you still have to go in and re-mate the parts you are pasting. Lots of work.

And so I reasoned, that, if I could create a part with multiple rotated configurations, and, that, if these rotated configurations are all driven by a single sketch ... then, it's not as much of a kludge because it's still like having a single part. There's only one defining element and every rotated configuration changes if you edit the parent sketch. The circular step-and-repeat approach suggested by Corey seems to be the way to go (thanks Corey). I have to test it further to be sure that it won't break with manipulation/changes.

Still bad logic?

-Martin

Offhand I would say, use a derived sketch. It will remained tied to the original sketches dimensions and relations.

On the other hand why not drive the original sketch from a design table or configuration specific dimension?

There is a component array feature. Check it out. If the 60 parts are inline you can array them in a single step. You can remove instances if there is a gap somewhere. If there are 2 levels of spokes put in each level and array them together.

Corey

curious logic... but logical! :-)

Actually, I do follow, and I understand how you got where you got. As Corey says, component arrays are wonderful things.

Again, I do not recommend it, but... if you want to do the sketch routine, here is what I suggest:

Since the part apparently has a center and spokes, create the first, or layout sketch with (for example), a vertical construction line from the origin, and one at whatever angle (but not constrained) from the origin (not constrained to verical or horizontal, just the rotation end point). Give these two lines an angle dimension. Construct other aspects of you basic part, but be sure that the sketch is constrained to these original 2 lines and center point such that a dimension defining the angle rotates the rest of the sketch. You can easily test this by changing the angle dimension. extrude your base feature. Then in each configuration, you only have to change the one angle dimension. That way there is no duplication of sketches or features.

Cheers, Daniel

Hey, curious-logical I'll take. There's enough curious to battle with SW, it seems, that if you have something that works you should go with it.

The prior suggestion to go with step-and-repeat worked like a charm. Now three configurations of a part are entirely controlled from the first sketch --as if it were a single config part. Thanks again.

-Martin