Ball bearing mated to plate follow a curved path

[Callesson]

Hello!

I would like my ball beaing follow a curved path/part. At the same time this ball bearing is connected to my plate.

Below is the bearing conncected to the plate. 

 

Here is the curved part

 

I tried the transitional constraint on the round part of the rail. And it did stop where the round part stoped. I want it to follow the straight line aswell. 

Also I could'nt constrain the mid axis of my ball bearing to a axis on the plate while having the transitional constrain on. 

Looking forward for help 🙂

[JDMather]

Attach your assembly here.

Do you have Inventor Professional with Environments>Dynamic Simulation?

[karthur1 · Accepted solution]

Create a sketch that the outside of the bearing will follow.  Extrude this as a surface.

Place this part in your assembly and use the translation constraint to attach the bearing to it.  You will have to set a view rep or just turn the visibility off for the path.

http://screencast.com/t/J9wqdhEB

Kirk

[Callesson]

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@Anonymous wrote:

Attach your assembly here.

Do you have Inventor Professional with Environments>Dynamic Simulation?

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Hi!

Thx for respond!

I can't send to the whole assembly but ill send you a dummy with these parts included. 

When I did put this dummy here I managed to succed with following the path. Using the transitional. But, maybe you could check if i've done it the right way. 

And in my real assembly I also managed to solve this. Instead of first mating my ball bear to the plate then after do the transitional, I FIRST did the Transitional then mated the ball bear to the plate. 

And for some reason that worked. Cause before i got the error " Constrain conflicts with another constrain kinda error" 

What could be usefull is to have som restrictions how far it can roll?(If thats posible) Also, could you do something like this but only using a simple LINE?

No, I do not seem to have dynamic SImulation!

Thx again 🙂 I have atteched the file incase you have time to look in to it. 

[Callesson]

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@karthur1 wrote:

Create a sketch that the outside of the bearing will follow.  Extrude this as a surface.

Place this part in your assembly and use the translation constraint to attach the bearing to it.  You will have to set a view rep or just turn the visibility off for the path.

http://screencast.com/t/J9wqdhEB

Kirk

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Very nice there Kirk!

You answerd my quesition there about the useage of just a LINE. (making it to a surface is clever)

However i'm getting some problems here. Its kinda like, sometimes it works and sometimes it doesnt. And also it wont follow the whole line. Only the part of the line i select.

Error is Attached.

Thanks! 

[karthur1]

The path does not have to be just a LINE.  It can be arcs, circles, lines, fillets.... etc.  Just when you extrude it, extrude as a surface, not a solid.

For the error, make sure the roller is constrained to another plane/surface that is normal to the curve.  Otherwise, Inventor will not be able to solve it.

Here is a video showing what I mean about the constraint.

I attached a simple assembly, but just noticed you are using 2012, so you will not be able to open it.

If you are still having trouble, post a sample of your assembly.

Kirk

[Callesson]

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@karthur1 wrote:

The path does not have to be just a LINE.  It can be arcs, circles, lines, fillets.... etc.  Just when you extrude it, extrude as a surface, not a solid.

For the error, make sure the roller is constrained to another plane/surface that is normal to the curve.  Otherwise, Inventor will not be able to solve it.

Here is a video showing what I mean about the constraint.

I attached a simple assembly, but just noticed you are using 2012, so you will not be able to open it.

If you are still having trouble, post a sample of your assembly.

Kirk

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Hi!

I am using Inventor 2015, I forgot to update it on my signature! It's updated now!

What I ment with a LINE was, I curved line yes! Just not a solid part. 

I'll look into what you linked and attached Thanks!

I kinda got it to work now btw. 

Is there a way you can restric this so it wont go crazy if you pull it to long. I will show a picture of it in my next post. 

Thanks for now!

[karthur1]

Here is an example that has all the parts... Sorry about that.

As far as restricting it, I know what you are talking about... are you constraining the roller with a translation AND a flush or mate constraint back to another plane?  That should keep it from flipping to the other side of the curve.

Kirk

[Callesson]

Awesome! No problem man!

I'm not sure if I can constrain it with a flush or mate yet. But I will check it out. Cause other parts are connected to other parts.

I'll give you this assembly here in attachment that you can look at. That pretty much what I want. 

When you slide the part connected to the Line there this other part should move along this curv via a bearing.

But if I now play around in inventor with this it will snap and find the reverse side/constraint and kinda go crazy like the picture below 😛 

So if you could look at the **** I attached that would be gr8. Thank you very much 🙂 

Maybe there is another way to solve this?

[karthur1]

Sorry for the late response.

One way to keep it from getting all mixed up is to limit the travel for one of the components.  I did it by using a min/max Mate constraint on the "fästplåtlinjär" and the "Rail_Con".   I would post the assmebly back here, but I am using 2015.

Kirk

[Callesson]

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@karthur1 wrote:

Sorry for the late response.

One way to keep it from getting all mixed up is to limit the travel for one of the components.  I did it by using a min/max Mate constraint on the "fästplåtlinjär" and the "Rail_Con".   I would post the assmebly back here, but I am using 2015.

Kirk

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Don't worry about that! I'm just glad that u are helping me! 🙂 And I'm using Inventor 2015 aswell so you can send files to me w/o problems. 

But I don't really know if I can do as you did in my real assembly. 

So I'm attaching a sample here of the work in progress assambly im working on. So what I attach is what I'm working with. 

If you could take a look at it and see if you can restrict it in that one aswell it would be gr8. 

Cause it is same here. If I play around with it, it will suddenly pop to another surface and that's not good. 

Like this : ->

[karthur1]

That is a bit tricky to get to stay the way you want it.  What I did was add a surface extrusion to the banaihop KA.ipt  This makes the roller constrained on both sides as it moves around the track.  It is still not 100% and sometimes it gets flipped over.  When that happens, just suppress the constraints, reposition it, then unsuppress them and it should be good again.

You should be able to unzip the attached file and open the HelpInventor-KA.iam and all the parts should resolve.

Hope that helps.

Kirk

[Callesson]

Hi, thanks agian!

I'll look into it 🙂 

Shame, that there is no way to really make this 100% functional. 

But thank you for your help and time! 🙂

//calle