Hi,
I'm trying to trim (cut) the outer surface geometry of a part to match where it contacted a surface that was revolved 90 degrees around the parts axis. In the attached Part File, the part would be rotated around it's axis (yellow boss) 90 degrees and the outer surface of the part would be trimmed to match the contour of the red surface (similar to grinding the outer surface of the part with a cupped wheel while the part was rotated along it's axis 90 degrees). What is the best way to model this in Solidworks?
Thanks for your help!
SolidworksParts And Features
Do you want the Gray part trimmed??
This is pretty much the same idea as , but I used a surface cut.
I extended your revolve
and circular patterned
creating a boundary surface from the first two 'ridges'
then repeat the surface cut pattern
I have another idea, I'm gonna play with
Hi Paul and Newell,
I agree, using the "steps" to construct guide curves could be a valid option. I was hoping that there may be a cleaner way to do this but that may not be the case.
To answer your question regarding the functionality of the part- a rotating cam driven off the red surface will drive and rotate the grey part which is why I need to ensure the surfaces remain in an intimate contact.
In my opinion, a model with a somewhat organic surface such as this should be done entirely with surfacing. But I guess it depends on the designer. You could accomplish what you are after by using a series of sketches on the adjacent faces tangent to the step lowpoints as guide curves, since you know that would be a continuous arc (can be refined by increasing your pattern instance). Also using sketch elements to loft & cut with surfaces similar to what Paul suggested. Again, depends on how accurate you want to make it.
I would reiterate my initial question of what is it you are trying to create? Is the cutting surface dictated by something else? maybe knowing the desired end product can yield alternate modeling approaches.
Matt,.. you could create a loft/boundary... to interpolate this using the edges (image attached)... but again.. the revolve is very close as well.. +/-?.
Hi Newell,
I think you're on the right track- I created a solid based on the surface, created 50 circular patterns of the solid spaced evenly across 90 degrees, combined the solids and then used that to subtract from the original part ( CAD attached). This gives me roughly the correct geometry but the problem with this method is that the surface has steps in it. The part will be molded so I need the surface to be smooth. Is there a way to accomplish this geometry without the steps?
John,
If I understand your method correctly, it doesn't quite yield the correct geometry since you are only revolving a 2D "section" of the surface rather than the entire 3D surface. Attached is a model of the result based on how I interpreted your post.
Can you elaborate on what you are trying to create? I agree with with John's method. However I don't think it would yield the correct result as the outer edge of the cutting surface would leave a trace closer to the axis as it revolves. (see image: combine feat with thickened surface rotated & patterned x90 - crude but approximate if only revolving 90deg.) I can't think of a scenario where you would be grinding with the inside face of the wheel as opposed to the out tangent edge.
It is possible, just depends on the level of detail you're looking for..
In the Top view add a sketch that is centered with the yellow boss
Select the Circle Sketch Point, Top Plane and add a plane
Add a sketch to the new plane
Select the Axis and Revolve Cut
You'll need to adjust your sketch accordingly..
Did you try to do an assembly with multiple parts rather then the single part..
Yes, that is the goal- To have the outer surface of the grey part trimmed to match the surface created by revolving the red surface 90 degrees around the axis (yellow boss) of the grey part.