Autodesk Inventor

[#1]

What instances is it necessary to combine 3d sketches with 2d sketches, I have used this combination a few times where I have to build rectangular frames then apply frame generator to the sketches to construct the frame members. I was told when I originally had training on Inventor 2013 that 3d sketches should be avoided where possible. Thanks

[#2 · Accepted solution]

Hi Anthony,

One general tip that might help is to know that you needn't have sketches to use the FG  (Frame Generator). Instead you can create a solid that defines the shape of your frame and use the edges to place frame members. FG automatically projects the geometry into the skeleton file that it creates using the selected edges.

For instance if you were trying to create this frame:

 

You could just create a solid like this, by extruding at an angle or lofting from the top profile to the bottom, rather than creating the "stick" frame 3D sketch.

 

If you need more edges you can sketch on the faces of the solid:

Using this method creates a more robust skeleton and is generally very quick to create and update.

There are time though where a 3d Sketch is needed, but I most often use them to work with 2D geometry that was created with 2Dsketches.

Here are some examples:

3D Sketch From two planar curves

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/3320-Show_Me_3320/3321-Show_Me_3321/3538-3D_Sket...

3D Sketch From intersection

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/3320-Show_Me_3320/3321-Show_Me_3321/3538-3D_Sket...

3D Sketch Wrap to face

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/3320-Show_Me_3320/3321-Show_Me_3321/3538-3D_Sket...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[#3]

Hello and thank you very much for your most helpful reply. I was not aware that FG may be used on solid bodies  so this will no doubt be extremely beneficial in future work. I will certainly make use of this technique now you have kindly pointed it out. May I ask, how would the solid feature be treated by Inventor once the frame generator has been used on it's edges ? I would guess that the solid would either be removed or would need to be suppressed in the tree ? Thanks again.

[#4]

I try to stick with surfaces (no solid bodies) in skeleon files, just to make sure I don't accidentally add any extra mass to the assembly.  One thing I don't like about this method over sketch geometry, though, is that I have to keep turning off the visibility of the skeleton surface in order to quickly select the frame members inside (otherwise, I have to right click and "select other" for each frame member), and turn the visibility back on to add new frame members.

The surface method makes it really easy to subdivide the frame, though.  For instance, to add horizontal beams around the perimenter of the frame 12 inches off the floor, just  offset a workplane by 12 inches, and use the split face tool.

[#5]

Hi Anthony,

You can just set the Skeleton part to be a Reference part and then turn off it's visibility and it will not show up in the Bill of Materials, the Drawing, etc. Setting the part to Reference also ensures that it won't impact the overall mass of the assembly.

You can do this if you use a 3D soild or some combinatiion of sketches.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com