3DSketch lines not parallel to principle axes 2

[MechDesg]

SW2006 sp 1.0

I am trying to use a 3DSketch in a "new part" in the context of an assembly. This 3d line will become the basis for a sweep that will represent a 1/4" O.D. air line. The problem is that every time I create the 3DSketch within the assembly (using the TAB to alternate between the various planes) the final result is not parallel to any of the planes. The part as a whole retains perpendicularity to itself but not the overall assembly that it was created within. Has anyone seen this before?

 

[ctopher]

When you create the new part, you selected a plane. Is the plane parallel to how you want it?

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[CorBlimeyLimey]

Instead of creating the part in the assy, create it as a separate part (with or without geometry) and then insert it into the assy using the standard reference planes. Geometry can then be added to the part using the ref planes and origin of the new part.

This will prevent the "in-place" mates and (IMO) will make for a more stable assy.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[MechDesg]

Thank you both for the tips. I tried creating the 3DSketch again but this time picked a different plane and it did work as I expected. So, is it the case that the plane to which you would like to initially parallel is the plane that you should select when you initiate this command? I've been a bit confused by this set of commands operate. Specifically, I am creating tubing routes in my top level assembly. I typically select insert-->component--> New part, the Saveas dialog box pops up, I create a new part file then it asks me to select a plane. Until today, I had been selecting any plane in the area of my start point that happened to be parallel to one of the principle axes. Now at this point the selection I need is "3DSketch" and then "line" but those are grayed out. So what I have been doing is: Select the Sketch dropdown on the command manager, select the sketch on the dropdown (first line) - which always pops up the what's wrong box and now the grayed out commands are selectable and I can select "3dSketch" then "Line" and draw my lines parallel to the axes denoted as XY, YZ or ZX. Does it sound like I am following the correct path here?

 

[rfus]

If 3d sketch is not working for you, you can combine multiple 2d sketches into a composite curve and use this as the path for your sweep. Insert -> curve -> composite and select the sketches.

RFUS

 

[ctopher]

Your steps are correct. When the line command is greyed out, try rebuild and see if it turns on.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[DanielGraham]

To expand on this...I think that some good points have been made, but the best feature of a 3D Sketch for 2006 has not been mentioned. You can make any series of planes that you want to reference for orientation before you start your 3D Sketch (or you can make the planes while in the sketch, but I will try to keep this simple.) Now you start the 3D Sketch and if you double click on a reference plane, then your sketch will behave more like a 2d sketch and all geometry will be limited to that plane (no need for tab). Double click on another plane to switch to that, or in space to revert to the old ways. Hope this makes sence. It made 3D Sketching much more powerful for me and eliminated me for using the old multiple 2D Sketch methods mentioned.

Daniel