intersection line missing in 2D engineering drawing

[skiwindsurf]

I found that the intersection lines are missing in 2D engineering drawing. In 3D models the missing of intersection lines are acceptable due to the shade difference of two bodies, but in 2D engineering drawing, it is very obvious. Any way to correct it?

Thanks. This forum is very helpful. And I hope you are not annoyed by this kind of basic questions.

 

[CorBlimeyLimey]

If the missing intersecting lines are between a screw shaft (at max thread dia) & a tapping size hole, then there is no "flick-of-a-switch" option to show the intersection. A cosmetic thread is often enough to indicate the intersection.

However, if you need a solid demarkation, you could add a 120° csk to the hole. The csk should be the same dia or slightly larger than the thread OD ... so that the edge shows. It would also represent the lead-in of the thread.

Give further details, or post a screenshot, if the above is not the case.


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[skiwindsurf]

My case is similar to the following:
A = sphere surface body of radius 1 center at origin
B = cylinder surface body of radius 0.5 and length of 2 center at origin

A and B would have 2 intersection lines. That is the intersection line I am looking for, but is missing in 2D engineering drawing

 

[ctopher]

Maybe show tangent lines in the view?

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

 

[CorBlimeyLimey]

You could use the Intersection Curve tool to create a 3D sketch of the intersections & have that sketch showing in the drawing views.

Or, you could use the Trim Surfaces tool to cut away the surface cylinder from inside the sphere, then the intersection lines will show.


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[bvanhiel]

If this is an assembly, then the behavior is normal. One fix is to cut a hole in the sphere so that the bodies don't overlap.

If this is in a part, then I suspect that you have two bodies that are not merged. If you merge them the line will be present.

-b

 

[skiwindsurf]

In my case this is an assembly, the sphere and cylinder are both components (In reality they are both more complicated than sphere and cylinder). It seems Surface Trims can only be used in a part. Can I use one component (which is a surface body) to trim another component in a assembly?

The intersection curve can be used to generate a curve, but to display this curve I would also need to turn all other sketches on, which is not desired.

So it seems no solution now.

 

[bvanhiel]

If you're just trying to "get-r-done" then you could insert the cylinder part into the sphere part as a separate body and do a body subtract.

-b

 

[CorBlimeyLimey]

OK, first question ... Why are you creating engineering (manufacturing ?) drawings of surface parts in an assy? Please explain (or show screenshot) of what are you are really trying to do?

Second ... Why do you need to turn all other sketches on to display the intersection curve? Individual sketches can be shown in a drawing view ... just expand the feature, RMB click on the sketch & select Show.


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[skiwindsurf]

first question: I am trying to get some patent drawings for a 3D machine.

second question: it is true that each sketch can be individually adjusted, I just learned this. The trouble with this is that, sketch line will be always regardless of viewing angle.

I think the fundamental issue is that I was trying to "cheat" the software by overlapping two surface bodies in space. So I took a step back, and really dug out a cylinder out of the sphere before putting them together.

 

[CorBlimeyLimey]

skiwindsurf ... FYI, using the Drawing View Manager (not the model Feature Manager) you can select and show an individual sketch in an individual drawing view. It will not affect the display state of the sketch in the model.


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