Bone Modelling

[rspoerri]

Hi

As a beginner of solid works I am trying to solve simple solid works
problems for my master thesis. what i have is the outer surface of the
bone and an inner surface. in the feature manager i can see both these
parts as inlet and outlet bodyvolumes. what I am trying now is to fill the
inner volume (and assign this solid body certain properties) and the same
for the volume inbetween the outer and inner bodysurface. seems pretty
easy, but I have no clue where to start! i have two volumes and would like
to have one solid body with a inner core material and a second layer
material (spongiosa bone and cortical bone).

i thank everyone in advance for any help

kindly

robert

 

[jimshaw]

robert,


First, welcome to mcadcentral.


Second, are these two surfaces bodies within a single part, or two surface parts within an assembly? It is unclear from your description.


What you are doing sounds quite easy, but we need a better idea of what you are starting out with. Can you upload the file? If not, then how about a picture/cross-section?


If you want different densities in the CAD, you'll need two separate parts in an assembly. If you're going to import this to an analysis and assign it two different mat props there, you might be able to keep it as a single part with multiple bodies. We'll need a little more info to go further, though...


Jim
http://www.linkedin.com/in/shawengineering

 

[jimshaw]

robert,


For quick reference, if you have an enclosed surface in a part, you can thicken it (Insert>Boss/Base>Thicken...) and when you select the surface, you should get an option to "create solid from enclosed volume". See here:


View attachment 5869


On the second one, you should get a "merge result option", which you should uncheck to leave the solid bodies separate:


View attachment 5870


Jim
http://www.linkedin.com/in/shawengineering
Edited by: jimshaw

 

[rspoerri]

Thanks for your quick reply.


Well the problem looks like this: It is an assembly ("Femur") which includes two components (outleft and inleft). the later two are the two surfaces, outer bone surface and the inner is the border between the hard bone and the soft bone.


Since the two surfaces are not "parallel"/"concentric", thus the internal surface differs form the outer", I can use the thickening function.


So what I want is to get a single assembly with an inner core of soft material surrounded by shell of harder material. (The shell as explained has not the same thickness all over).


When I finish this part I will cut the head of the bone in order to simulate a fracture and position a second assembly (a screw assembly out of 4 parts) in this femur. to make it short. I want to simulate a bone fracture and see how load are distributed after introducing the screw implant in the broken femur model. Does this helps enough?


Thanks again

 

[jimshaw]

robert,


Yes, this makes perfect sense. Reread my post, as I am not suggesting to use the "thicken" function in it's fundamantal sense, rather to use it to "solidify" an enclosed surface.


Here I have a cross-section of my test assembly, with the inner green "soft bone" enclosed surface floating inside of my outer orange "hard bone" surface. You can see that the distance between the two is not constant due to their shapes. The first pic shows them as surfaces, the second pic shows the inner bone "solidified" using the thicken feature as described above, and the third shows the outer bone "solidified" using the thicken feature as well.


View attachment 5871View attachment 5872View attachment 5873


However, the inner bone volume is now occupied by both parts (notice the orange smudges in the middle of the inner bone part?), and this won't work with FEA, so we need to perform a boolean operation to "hollow out" the outer bone. To do this:


1. From the assembly, right-click on the outer bone and select "edit part"
2. Select Insert>Feature>Cavity...
3. Expand the component tree and select the inner bone part for the "design component, then select OK
4. Gain control of the assembly again by right-clicking on the assembly icon at the top of the component tree and select edit assembly.
It should now look like the picture below left, notice the orange smudges are gone. Turning the cross-section off, we see the finalbone assembly (below middle).And finally, we open up the outer bone part and make it transparent to verify the cavity; it should look like the pic below right.


View attachment 5874View attachment 5875View attachment 5876


There are other ways to hallow out the outer bone, but I believe this is the cleanest, and most parametric ("best practice"). At this point, you can import the geometry into your FEA tool, and assign independant mass props to each volume, mesh, solve, etc.


Can you repeat what I've done on your assembly?


Jim
http://www.linkedin.com/in/shawengineering

 

[rspoerri]

sounds easy thank you very much.


in the mean time I have a new problem. my university did not renew the licence for an up to date solid works software package. they switched to inventor.


now I have the same problem, I have an assembly with two surfaces. but I dont see any thickening function for them. according to tutoriakls it would be quite easy to find this function under modell - area - thicken. why dont I see it? did I import a unvalid file type ( I tried with IGES or prt)





Thanks again