3d sketch in assembly
3d sketch in assembly
(OP)
Could someone give me clarificaion on this matter. I'm trying to create a 3d sketch in an assembly (SW 2001 plus). I selected my face to start my spline and I want to end my spline on another face on another face. I can't see that face in the current view(iso). To see the other face I rotate my view to see it, but it changes my spline path. What am I doing wrong. Thanks for you help.
Derrick Langley
Derrick Langley






RE: 3d sketch in assembly
Instead of points, you might use reference lines with one endpoint coincident with the face and the line constrained perpendicular (normal) to the face. This comes in handy if you are trying to control spline direction where it meets the face.
Also, many times it seems easier to just "throw in" a 2- or 3-point spline, then move the ends to where I want them. Keep in mind that you can also add or remove interior spline points as needed.
And I'm available for consultation,
but remember your way in is also my way out
RE: 3d sketch in assembly
Derrick Langley
RE: 3d sketch in assembly
But to get back to 3D Sketch - when you make a 3D Sketch it may look like it is where you want it but it puts it in according to the X,Y,Z coordinates. You will see that when your dropping your points. Most of the time it puts the spline in X,Y. You have to adjust the spline or use your Tab key to give it some direction like X,Z so on so forth. Dropping in a 3D spline isn't cut and dry like it is with a 2d sketch spline. You have to be crafted with it. Use lots of Relationships to help control the spline. Drag the points around to help control it. Once the spline is in even though it may not be in the direction you want it the time. You should put relationships to the end points to be on both surfaces (preferably to a point from a previous sketch, this gives full defintion of that point). then look at the front view and drag the points to where you want them. Then look at the right do the same thing, then the top, etc... you will eventually get it where you want it. Splines are harder to work with then lines, IMO.
IHTH - if you followed it,
Scott Baugh, CSWP

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RE: 3d sketch in assembly
It also helps to get acquainted with the "pierce" sketch constraint. This allows you to constrain to the point where a curve intersects the sketch plane.
RE: 3d sketch in assembly
Derrick Langley