Mating surfaces 3

[OptiEng]

Hello all,

I am trying to mate the exterior ball surface to the internal surface of the cup in the pelvis. I have tried all sorts but had no success. I have tried creating reference points and also different mating options but need some help. Can anyone offer any advice? I am using solidworks 2005, but also have access to solidworks 2009 if needed. I have uploaded an image at

http://my.engineering.com/pg/file/OptiEng

called CAD Model 1.

Thanks

 

[EEnd]

How about putting points at the center of both spherical surfaces and using a coincident mate?

Eric

 

[CorBlimeyLimey]

Do you get an error message when creating the mate?

Are other mates preventing the mating of the spherical features?

 

[OptiEng]

Hi, thanks for your feedback.

EEnd, yes I have tried this... please find attached another picture called CAD Model 2 at

http://my.engineering.com/pg/file/OptiEng

showing creating the two points, I can select point 4 but it will not let me select more than one point. Any suggestions? Thanks.

 

[steinmini]

I would try to mate the point in the ball (sphere) via "distance" to the specified point in the cup. Coincident will most likely not be accepted between the two surfaces; did something similar and the only way I could mate the sphere and the cup was with distance between the center point of the sphere and the surface of the cup - a half of a sphere as well. The distance should keep the sphere at the end of the bone always at the same distance from the defined point on the cup's surface and allow movement around the point within the sphere. If that point is not exactly at the center of the sphere, well, then it should be placed to the exact center...

 

[rstupplebeen]

Try mating points that are in the sketches of the 2 parts not points that are in the assembly. I hope this helps.

Rob Stupplebeen

 

[CorBlimeyLimey]

If the cup and ball of the joint are truly spherical, selecting the surfaces and the Concentric mate option should work. If it doesn't, you may have other mates (or constraints) preventing it. If that's not the case, you may have deeper problems.

 

[Theophilus]

I've done this with sketch points just fine before (as Rob and others have suggested). It works fine, whether actual origins of parts or points within sketches (such as the center of a revolve feature) to constrain two spheres concentrically.

Make sure your sketches are visible so you can select the points, or if your origins are concentric to the spheres, select them in the feature tree.



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.

 

[OptiEng]

Problem solved thanks everyone!

 

[CorBlimeyLimey]

Care to share the solution for future reference?

 

[EEnd]

To elaborate on what rstupplebeen said... The points should be made in the corresponding parts, not in the assembly.

Eric

 

[OptiEng]

Yes this as EEnd and rstupplebeen mentioned it was just a case of defining the points in the individual part files and not the assembly.

FYI This is how I did this. From the assembly I opened up each of the two parts and added a reference point to the centre of the ball (using the arc centre option) and a reference point on the cup (again using the arc centre option), then back in the assembly, I mated the two piont together (coincident) by selecting the two point from the assembly tree.

Thanks again everyone.