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Im new to solidworks.. what im tring to do is create a working spherical bearing.. when i try to mate these 2 spherical shapes it doesnt give me a choice on a type.. of mate.. any sugestions? Thanks TOM
You could try a cam mate under advanced mates, or the simplest way would be a distance mate of the radius from the center of the spheres. If you have the planes in a good place, just mate the plane as necessary.
Simply do a coincident mate to the centers of the two spherical
features. If you're inserting this bearing into another assembly,
remember to set it to "flexible" for it to allow the ball to pivot in
the socket.
I'm having the same problem and have now spent about 2 days trying to resolve this. I am trying to insert a bearing into another spherical shape.
Most of the mates do not work , for example you cannot highlight the outside of the bearing in order to create a mate.
From the above, i understand that if i can mate the dead centre of both spheres and then create a distance - this would possibly work.
Can someone, please - PLEASE! take me through step by step on what options i need to click on to highlight the centre of the spheres and then create suitable mates - to make this work
Also, when i right click on a part i only ever seem to have the option to FIX not FLEXIBLE -
You can insert as many planes as you wish with specific angles, distances... And they could help you in mating. If not, let me know, I ll try to help, I'm in a hurry now!
1. You can mate "concentric" for two spherical faces, if you make a spherical sliding bearing. Click "mate", "concentric" and both spheres.
2. You can mate "tangent" for two spherical faces. It is necessary to add mate "distance" between origin of one part and some planes of other part. You can clickan origin in design tree.
3. You can use a mating of origin of parts, if this points coincident whith a center of spheres. Click "mate", open parts in design tree, click "origin" of both parts. You can use mates: "coincident" and "distance"
4. Do references points in PARTS, which have spherical face:
Reference geometry => Point => center of face => click on spherical face. This method is applicable, if you have no origin in center of spheres.
Use other faces or planes for additional orientation.
Other mates are used very rarely.
Also, when i right click on a part i only ever seem to have the option to FIX not FLEXIBLE
If you insert assembly 1to assembly 2, parts, which move in assem 1, cannot move in assem 2 default. Right click on an assem 1 => Component property => Flexible. Parts have "FIX" or "FLOAT" only.
I will be able to help anymore, if you will expound aproblem more concrete.
Thank yoi to everyone that took time to respond to this
After some guessing and gambling with different aspects I have succeded in resolving this
Firstly - ensure that you create the Origin at the dead centre of the sphere - so with the extrusion change one of the options so that the extrusion starts from the mid point
Once you have this for both parts you can you to the menu/view and choose to show "Origin"
You can then click on each origin and use these to mate
In your assembly make a circle sketch with the center in center of the cageand mate the center of the sphere coincident with the sketch. You can addsome relations between the sketch and cage of the bearing
If your part is allready created and you can't make the origin the center of your part (centering your origin isthe best way to do it) you can also create points at the center of your spherical items and constrain using those points. (I did that yesterday with some old models that weren't drawn with the center at origin how timely!)
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