2Dto3D - thickness

[MikeHalloran]

I'm converting, okay trying to convert, a fairly complex set of curves (3 views of an engine) to solids, with some difficulty.

One thing that bothers me, in trying to extrude (within the conversion toolbar), is that SW has a strong preference for making the solid 'thin'. I.e., it comes up with 'thin section' checked, greyed, and unchangeable. I, personally, have no preference, but the 'thin' seems to cause build errors that prevent completion of the solid. Last week, I managed to change the dialog to 'not thin', and the polygon extruded beautifully and all that.

Anybody got clues for how to deal with SW in this corner of its capabilities?



Mike Halloran
Pembroke Pines, FL, USA

 

[MikeHalloran]

E.g.: "Unable to create a thin feature in the specified direction. Please try a smaller thickness."

Ok, the polygon has some small steps in it. I'll try making the thickness smaller than that.
Nope; went down in thickness from 0.1 to .002", no change.
Tried extrude blind instead of extrude between vertices (neither in the sketch plane), no change.





Mike Halloran
Pembroke Pines, FL, USA

 

[TheTick]

I never use the actual imported sketches for conversioin. Too many chances for error. Usually I use the imported sketches as master sketches and use them to copy entities or constrain.

 

[Theophilus]

Exactly--if the sketch has any breaks or duplications in it (which, if done in 2D, it most likely does have) then you'll only be able to extrude a thin feature without repairing the sketch. Because if this, I also create my own sketches with imported sketches as reference.



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.

 

[CorBlimeyLimey]

usually the Thin Feature option only becomes selected and unchangeable when the profile being extruded is an open loop.

 

[MikeHalloran]

What I've been able to do so far is start within the imported sketch, pick some related entities and attempt an extrude. If I pick few enough, I can get a successful extrude of _something_ in the right direction.

As a side effect, that extrude produces a new sketch. I delete the extrude, then edit the sketch by converting or overlaying the lines that I really want to extrude, and using that sketch as the basis for a new extrude (from the solids toolbar, not the 2Dx3D toolbar).

.. which is _not_ how the 2Dx3D tools are supposed to work, if I'm reading correctly.

Yesterday, while screwing around with trying to actually use the tool as documented, I got a yellow preview of a short thin extrude that had the thickness of an arc going the wrong way somehow. That selection/subsketch/whatever would never extrude properly, but I thought there was a clue there; i.e. extruding per the preview would make a Mobius strip. But I couldn't find a way to edit the components (of the imported sketch) to make it work differently.



Mike Halloran
Pembroke Pines, FL, USA

 

[mjcole]

Mike,

Tools > Sketch Tools > Check sketch for feature
Is a good thing to use to verify the sketch for a specefic feature type.
It will show you open loops and overlapping entities and other problems. In 2009 there is a local zoom window but it sometimes helps to hide it.

Another way to find open loops is to Right click any Sketch entity and Use Select Chain. If there is an ambiguous solution more than one path then you can change an entity to construction or delete it.

To steal (borrow) from Robert Frost's "The Road Not Taken" and translate it into SolidWorksSpeech.

"Three lines converged at a point,
and I deleted the one of lesser length,
and that has made all the difference."

Another trick for investigating the converted sketch is to select all the geometry with a selection rectangle and select and highlight each one in the list Line1, Line2, Arc3 etc. and look for duplicate highlights on same entity which is a lot easier than using Select Other and right clicking each entity. Select Chain is a more direct approach to finding broken open areas.

When you use 2Dx3D wizard you are forced to select Front Sketch first then you get the others. But when selecting geometry from import there may be overlapping entities. You can use this tool with my previous investigation techniques to clean up the sketches.

Another option is to use selected contours option in extrude tool to pick a region of the sketch. This works for bounded areas and closed loops Rectangles, Circles. If you had a Thin Pipe you could pick the Outer and Inner Circle, or Select the area between them.

Michael