I'm trying to offset a section of pipe using two 45 degree elbows. I've attached a test sketch, I have two sketches one uses a plane and it works as I need it to, the second is trying to use a 3D sketch however no matter what I try it keeps saying it's over defined. Anyone know how to make this work?
I don't understand your end result if both are used to Route, but I think I understand that you are moving from one end point to another.
Regardless of intent, here is how I achieved error-less 3D Sketch.
Delete Colinear14 and Angle31. (selected in blue)
Then add AlongX relation between these two points.
Result, shown from top:
Does that work for your intent?
Sorry I should have been a little clear, I'm just trying to make the 3D sketch, not using the plane.
I have both sketches to show that it is possible however ever I can not duplicate the same result just using a 3D sketch. I can get it to work if I don't have the lines tangent however that doesn't provide a proper result.
Does that make more sense?
Yes. You want to recreate 1st sketch as 3D sketch, without relations added to first sketch, so that you can abandon 1st sketch and carry on with 3DSketch. I will try this tomorrow; sorry out of time today. My first idea is to remove some dims and set arc and angle related to the other dimensioned one as equal. Other is to replace colinear with coincident to a point, whereas I had removed it previously.
Ya, I've tried many different ways and can't seem to get it to work unless I use the plane however when I try using the plane in the actual routing file it's giving me the errors. Thanks for looking into this.
I deleted these in blue: radius dim, angle dim, colinear.
I added coincident from the upper line to the point below (replacing colinear).
I set both arcs to equal (replacing deleted radius dim).
To check the design, I placed a reference dim where the angle dim was. Though driven, it checks as 45.00º.
Ya that works, I guess solidworks doesn't like you actually having both dimensioned. Thanks for the help I greatly appreciate it.
I wouldn't jump to conclusion towards a rule such as do-this-don't-do-that, other than sometimes 3D Sketches behave illogically to create OD errors when it shouldn't.
Odd behavior in 3D Sketches comes along with the flexibility of the tool, such as taking a FD sketch, deleting one relation, and getting an OD sketch. It doesn't make any sense at all and doesn't get a reason to apply to it. Nonsense is a reasoned conclusion, as we try to make the best of it.
I agree, I find a lot of odd behavior adding these into piping routes, which is a completely different beast on it's own.
I deleted these in blue: radius dim, angle dim, colinear.
I added coincident from the upper line to the point below (replacing colinear).
I set both arcs to equal (replacing deleted radius dim).
To check the design, I placed a reference dim where the angle dim was. Though driven, it checks as 45.00º.