3d sketch in assembly

[ddlangley]

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

 

[TheTick]

I find that when creating splines, especially in 3D, it helps to put down some anchor points first. Sketch a couple points and constrain them to the faces of interest, and use those as guides.

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.

There's no double-lock defense; there's no chain on my door.
And I'm available for consultation,
but remember your way in is also my way out

 

[ddlangley]

Thanks Tick that did work, but how do I now create a sweep along that spline so I looks like a hose. Thanks once again.
Derrick Langley

 

[SBaugh]

If your in an assembly and making a assembly sketch you realize you can't extrude in an asembly sketch, only cut. If you want to create a part between the two other components you have to add a new part.

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
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

Create a datum plane using "normal to curve" and selecting the endpoint of the spline and the spline curve. It helps to set the plane origin on the curve (checkbox below option button in datum plane menu). Use that plane to sketch your cross-section.

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.

 

[ddlangley]

I just want to thank all of you for your help. Taking a little advice from every response got me on the right track. Thanks once again for taking the time out to answer my post.
Derrick Langley