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Contact Problem between parts in an assembly

Contact Problem between parts in an assembly

Contact Problem between parts in an assembly

(OP)
I am trying to get an assembly model to mate.  The models consists of a helical gear - constructed using the helix curve method in solidworks, a pin and a ball.

All that I am trying to do is position the pins and balls to contact the tooth flanks of the helical gear in a similar way as what a real pin or ball does during measurment of the helical gear.  ie a measurment over pin or ball method.

Solidworks 2009 will not let me mate the parts with tangent surfaces.  Is there a different way to do it accurately?

A zip file of my models are attached

RE: Contact Problem between parts in an assembly

I have not gone thru your files but try splitting the surface of the ball into 2 or 4 parts.

Another way can be to mate with sketches.

I am no Gear expert but I am not sure about using pins as I thought pins can not be used on helix gears.  

RE: Contact Problem between parts in an assembly

(OP)
Gurjeet

Balls and pins are standard ways of measuring helical gears in the gearing world.  When I draw spur gears using the same technique, solidworks works fine.  Its only when I apply a helix, that this sort of problem happens.  Sometimes I can make one surface tangent to a pin, but it cannot lock onto a 2nd surface.  I have never been able to get the balls to contact on any surface.


I tried splitting the ball into something that looks more like two hemispheres with a rod in-between - the same result - it wont contact


Anyone have a different suggestion?

 

RE: Contact Problem between parts in an assembly

You can do a combination of types of mates.  If you need the ball to be a certain distance from the front face then do a distance mate on the planes.  Then you can do a Move with Physical Dynamics turned on to nest the ball in the groove.  When the ball stops (contacts the groove) you can do a Fix mate to keep it there.  Otherwise you will have to get creative with putting a point sketch at the center of the ball and making a curve that follows the helical cut at the right position so you can mate the sketches.

Dan

www.eltronresearch.com
Dan's Blog

RE: Contact Problem between parts in an assembly

(OP)
Dan

What I am trying to do is not just create a nice picture, but to gain some data in the process.

Creating sketches and curves presupposes the solution to the problem and then just postions things there.

When you physically do this on a part in the real world, the ball or pin just sits on its own in the right spot - there is only one real world solution.  The fact that solidworks 2009 cannot find that solution is kind of frustrating.

The solution using physical dynamics to find the contact point doesnt work very well either because the ball has to contact on 2 points not 1; so finding that position using that technique doesnt really work either.  In the case of the pin, it has to contact on 4 points.  Easier to do in the real word than in Solidworks I guess.

Is there a different way to approach this?  Is this a feature that solidworks 2009 just cant handle?

RE: Contact Problem between parts in an assembly

Create surfaces offset from the gear at 1/2 the diam of the pin or ball. Create a curve at the intersection of the two surfaces. That will be where the axis of the pin or ball should be placed.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services
www.infotechpr.net

RE: Contact Problem between parts in an assembly

(OP)
Peter
This approach is worth exploring.  I can create the offset surface, but how do i create the curve at the intersection of the two surfaces?

I dont seem to be able to find anything on insert curve command that is appropriate.

I also notice that when i create an offset surface, even with a small offset - say .0001 mm, i still cannot use any mate options to mate the ball to the surface.

RE: Contact Problem between parts in an assembly

You'll have to start a 3D sketch and go to tools/sketch tools/intersection curve.  Or do a mutual trim of the surfaces and convert the edge.

Dan

www.eltronresearch.com
Dan's Blog

RE: Contact Problem between parts in an assembly

... or skip the Intersection Curve and just use the trimmed surface edge.

RE: Contact Problem between parts in an assembly

(OP)
I was able to trim the surface and then create a complex curve on the the trimmed edge. I then mated the center of the ball to this curve.

The results of this excersize was very interesting.

First of all, in the real world, when you measure a helical gear this way with balls, it doesnt matter where the balls are placed in relation to the face of the gear, as long as both balls are held in the same plane.  I constrained the balls that way in this assembly as well.

However the result I found in Solidworks using this technique did not match exactly to the real world.  If I place the balls with their centers on the curve described above precisely in the middle of the face width in the gear model, we have a very accurate result that matches the mathematical calculaton.  ie the dimension over the two balls matches theory within a fraction of a micron.

If however both balls are moved closer to one face, the distance over the balls changes dramatically - which does not happen in the real world.  In this particular example, the error became .03 mm measured close to one side than in the middle.

I suspect that the flaw in the method has to do with the assumption that we can just offset the surfaces by half the ball distance.

When we offset the surfaces by half the distance of the ball, it does not take into account that the ball does not touch both flanks in a plane parallel to the face.  On one side the contact is a little on one direction, and on the other side it is a little to the opposite direction.  Hence we are really not exactly portraying the precise location of the ball contact correctly.  This was further seen in my model example by a small visual gap between the ball and the tooth flanks after the center of the ball was placed on the curve.

A 2nd flaw could be in how solidworks creates a swept helical surface.  To verify this we would probably need to take surface points from the solidworks file and compare then to theory.

Does anyone have a different way to approach this problem? The fundamental issue is that we want to have the surface of the ball contact the tooth face on the model.  Solidworks wont let me do that with the model.  I have updated the link below to show the latest models including what I did with the offset surfaces and the balls.

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