How to 3D sketch not on a plane 2

[NCSU1980]

How can I 3D sketch, so the sketch is not on a plane? I am trying to sketch a wire that goes from one place to another in 3D space using the top down (in assembly) method. I am going from "near" one part to "near" another part. In Inventor or Pro-E I would create work points at the intersection of 3 planes, a plane and an axis, etc... and create the 3D sketch by going from one point to the next. I have done this in SW by going from one sketch point to the next. I would like to create work points (which seems to be a SW weakness, although I can create work axis and planes just fine)and go from one point to the next or free sketch the line and use relations to tie the end into 3 planes to locate it. Is there a way to do this? Am I missing some way easier to do this?

 

[TheTick]

Datum points in SW are indeed weak. I prefer to place point entities within a 3D sketch.

Perhaps use two separate 3D sketches? One for key points (I also include construction lines for wire direction at key points), and the second for your actual wire.

 

[NCSU1980]

Could you explain a little more about how to place point entities within a 3D sketch? I do not understand, since making the 3D sketch is what I am having trouble with. I am also having trouble grasping the two seperate sketches concept.

Thanks
Steve
SW2006 SP 5.0

 

[ctopher]

Draw a 3D Sketch, move the points where needed, create a sweep.

http://www.youtube.com/watch?v=9xAOjOLlCS8&feature=related

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08; CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[NomLaser]

Create a new part and just save it blank. Insert it into your assembly and mate the planes to the origin in the assembly. Now it is locked in space. Edit the new part while in the assembly and start a 3-D sketch. Insert points where you need them. Create spline between points how ever you desire. Exit the Edit Part mode and open the part separately. Now insert a plane normal to the curve. Now you can sketch a circle for your sweep then sweep the circle along your 3-D sketch. That's how I usually create flexible cables.

 

[NCSU1980]

DEddie, thanks. The light is getting brighter. I like your advise to start a new part and insert it. Instead of inserting a new part in the assembly from the drop down which immediately wants you to choose a face to sketch on, it lets you mate the planes first and then start a 3D sketch. Also the simple statement "insert points where you need them" made it clear to me. (Feature datum points from planes and axis would be better, but we work with what is available.)

Another question. Is there a way to make a segment of the spline between two spline points perfectally straight? I can do it by stopping the spline sketch.....then sketching a straight line between two sketch points.....then starting up the spline and finishing. But being able to just pick a segment you want straight would be easier.

 

[NomLaser]

I agree, though I don't know of a way. I usually try to use lines and arcs in 3d space because you can set them straight a long a direction and make them concentric with existing features in the assembly. My typical wire routes consist of making lines in the directions that I want then adding sketched fillets to add the arcs. I found that it's easier to align everything and splines can get messy in a hurry. You can also dimension the lines and arcs for easy modification. Let me know if you need me to post an example.

 

[NCSU1980]

I think I now understand 3D sketching with SW in context pretty well. Just have to do 3D sketch points instead of datum points. Can use existing features or can create planes or axis and put the sketch points on said plane or axis or a set distance from said feature, plane, or axis to locate it.

A question regarding the statement in the previous post about making the lines and arcs concentric with existing features. Does this just mean having an arc concentric around a round post or is there more I am missing?

Thanks again
Steve

 

[NomLaser]

Yes, when I normally create wires it is to a round pin hole or a pin itself and I start with a straight line from the pin or hole in a connector. I make that straight line concentric with an in-context relation to start with until I get the sketch laid out.

You can create the sketch with in-context relations. Then when you reopen the part to edit the sketches and create the sweep, you can break the relations if your company doesn't allow in-context relations to other parts. Many companies don't allow this due to being burnt in the past by having parts change unknowingly if another part changes.

I'll create a quick example of what I'm talking about.