How to Leave a Smooth Surface after Cutting from an Odd Geometry

[Phebotalus]

Hi, everyone.

I'm editing a model of an aorta in SolidWorks, and I need to cut off the some extra parts I do not need... Specifically, there are arteries coming off of the aorta. I need to somehow cut them off the main branch, but have the surface I cut them from be smooth after the cut. I was wondering if anybody had some ideas as to how I could do this.

Check out this image to see what I'm talking about:

https://www.healthbase.com/hb/images/cm/aorta.jpg.

There are arteries at the top, which in my model would need to be cut.

Any ideas or thoughts would be appreciated. Thanks,

Phebotalus

 

[NomLaser]

How is the aorta created? If it is a sweep you could do a sweep-cut the same diameter as the aorta. Without seeing the model it would be hard to really determine the best method.

 

[TheTick]

Use "Delete Face" to get rid of extra faces. You can even use it to plug holes.

 

[Eltron]

Have you tried doing a simple extruded cut with the "Up to Surface" end condition?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[ctopher]

Try "Trim Surface"?

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[bsj0526]

I would also try to do a knit surface on the aorta, and try to unitrim or extend the surface to fill in the holes where the arteries branched off. Then just do a cut with surface.

 

[Phebotalus]

NomLaser - It was created using the Scan3D function from a .stl mesh. It uses actual MRI data so it is not of constant diameter. I would have posted the model, but it's unfortunately confidential. I know it's hard to visualize what I'm describing without posting the model, :-(.

TheTick - Thanks, I'll try using that function.

Eltron - Yes, I have tried that. But since the model is composed of hundreds of surfaces all at odd angles to eachother, SolidWorks cannot calculate how to properly make the cut.

ctopher - The function seems to be disabled, I'm not sure why.

bsj0526 - Could you explain more what you are talking about? I'm not sure I'm quite following what you are thinking about.

 

[rstupplebeen]

Please check out the files because they will tell a better story than I can. But here goes.

I made a representative geometry by creating a boundary solid between 2 ellipses and a sweep of another ellipse and saved this out as an STL.

Imported the STL deleted the faces joining the main body to the other body and then did a body delete with the rest. Surface filled the hole and knitted into a solid.

On the other side I tried a different approach by doing an extruded cut then filled then did another extruded cut slightly smaller and did another fill. This was to contain the faceted surface to an annular ring (check out the curvature before and after).

I hope this helps and makes some sence.


ht

Rob Stupplebeen

 

[Georgels]

Phebotalus, It would be best to create surfaces from your scan data using a program like geomagic or imageware. Then you can edit the nurbs surfaces in Solidworks. Solidworks is not made to deal with scan data.

Also, 3d studio max or blender.org (free) could be used to edit these files.

George

 

[bsj0526]

Since your part is a scan, the aorta is probably made up of more that a couple of surfaces, so this may not work. But, I was suggesting that you select the surface(s) that make up the aorta, and use the knit surface feature to create a 0 offset surface of the outer aorta walls. There should be holes in the surface where the arteries branch off, but you can fill them in using either Unitrim or filled surface command. Then, you could just do a cut with surface and point it outward to remove the arteries.

 

[mjcole]

Scan to 3d allows you to smooth out the imported surface even if the data shows as sharp triangles like STL. You can edit the scanto3d feature if you have Premium and it will allow you to remove extra points that are inconsistent with the shape expected. Most of these surfaces show up as smooth patches. You will in some cases get many smaller surface patches amidst the smoother continuous portions.

If there is a way to get the STL in point cloud form the resulting shape will be a lot smoother.

Michael