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Changing location of gear tooth with gear's overall dimension

Question asked by Dan Cairns on Apr 5, 2019
Latest reply on Apr 8, 2019 by Dan Cairns

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See attached. I'm trying to update this part I've inherited and my task is to decrease the gear's overall dimension. The initial diameter was set by using revolve about an axis and then the teeth were created using the cut feature. When I decrease the size of the diameter to say, 15mm, the sketch for the cut doesn't move with it. The sketch has concentric and fixed relationships. Deleting those and trying to re-position the sketch so that the cut goes through the new revolved body doesn't work. I've attempted to add dimensions from the bottom and top of the sketch to the middle of the revolve; changing that doesn't do anything.

I can't figure out how to move this sketch if I decrease the diameter of the gear. Can anyone help? I've attached the part. Any help I can get would be great!

Kevin Chandler Apr 5, 2019 4:09 PM

Correct Answer

Dan Cairns wrote:

Yup, I have tried that and doing so seems to over define the sketch. There's a fixed relation at the bottom of the tooth but if I don't keep that it seemingly makes things worse.

Fix is generally a bad idea unless it's absolutely unavoidable (and it usually is. I see Fix as more of an indication that I got some more thinkin' to do).

Delete the Fix relation and try placing a dimension from the root to the midpoint of the arc (right click it and select midpoint) instead.

Your Plane3 has gone into the red, too.

I don't know what went missing, but these selections should remain after model edits:

After this, your M5 is still narfed up.

Like me, this dim appears to have lost its marbles somewhere.

But it's not needed, because you've correctly modeled at the origin and about the default planes (YEAH!!!), so delete the dim and the current point and add a new point at the origin.

Kevin

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07-01-0232.SLDPRT.zip206.1 KB

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Kevin Chandler Apr 5, 2019 2:45 PM

Hello,

In the upper right, click the magnifying glass icon and search the forum on gears and this topic has surfaced numerous times.

To address your OP, your relation is concentric.

It needs to be coradial to move with the OD change.

Kevin

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Dan Cairns @ Kevin Chandler on Apr 5, 2019 3:01 PM

I did look and wasn't finding someone else having this exact same issue, do you mind giving me an example?

Should I change the concentric relationship to a coradial one, or delete the concentric relationship entirely and create the coradial one from scratch? This will be interesting because the part was created with a revolve and not a circle + extrusion.

Thanks

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Kevin Chandler @ Dan Cairns on Apr 5, 2019 3:48 PM

Dan Cairns wrote:

I did look and wasn't finding someone else having this exact same issue, do you mind giving me an example?
Should I change the concentric relationship to a coradial one, or delete the concentric relationship entirely and create the coradial one from scratch? This will be interesting because the part was created with a revolve and not a circle + extrusion.

Thanks

Hello,

The search was just a reminder because there have been many gear posts and you may find search usual for other issues.

That typed, Delete the concentric at the OD and add a coradial with the tooth's arc and the OD's edge.

That should suffice (I believe).

Kevin

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Dan Cairns @ Kevin Chandler on Apr 5, 2019 3:55 PM

Yup, I have tried that and doing so seems to over define the sketch. There's a fixed relation at the bottom of the tooth but if I don't keep that it seemingly makes things worse.

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Kevin Chandler @ Dan Cairns on Apr 5, 2019 4:09 PM

Dan Cairns wrote:

Yup, I have tried that and doing so seems to over define the sketch. There's a fixed relation at the bottom of the tooth but if I don't keep that it seemingly makes things worse.

Fix is generally a bad idea unless it's absolutely unavoidable (and it usually is. I see Fix as more of an indication that I got some more thinkin' to do).

Delete the Fix relation and try placing a dimension from the root to the midpoint of the arc (right click it and select midpoint) instead.

Your Plane3 has gone into the red, too.

I don't know what went missing, but these selections should remain after model edits:

After this, your M5 is still narfed up.

Like me, this dim appears to have lost its marbles somewhere.

But it's not needed, because you've correctly modeled at the origin and about the default planes (YEAH!!!), so delete the dim and the current point and add a new point at the origin.

Kevin

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Dan Cairns @ Kevin Chandler on Apr 8, 2019 12:38 PM

Thank you!

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M. B. Apr 5, 2019 4:24 PM

Here is a method that does what you asked for but is probably not what you want if you want accurate gear teeth.

Assuming that you can't make changes to the tooth sketch, this will allow you to use the original sketch without modifying the tooth profile. I've added a derived sketch, 3 equations, and a few other minor sketch changes. Also added the R22.5 & R15 configurations.

Keep in mind that all this does is get you moving along with an inaccurate but pictorially correct gear. If you want an accurate tooth profile for different OD sizes, you will need to make significant additional modifications to the original sketch.

Attachments

07-01-0232.SLDPRT.zip571.5 KB

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Dennis Dohogne Apr 8, 2019 7:23 AM

Dan,

That model you are working with apparently was not made with a good plan toward changes. Here is a good parametric gear model I made. Just edit the Design Table and change the values in the three green columns.

Attachments

Involute Gear, Metric, DesignTable 2016.SLDPRT.zip432.6 KB

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8 Replies

Kevin Chandler Apr 5, 2019 2:45 PM
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Correct Answer
Hello,

In the upper right, click the magnifying glass icon and search the forum on gears and this topic has surfaced numerous times.

To address your OP, your relation is concentric.
It needs to be coradial to move with the OD change.

Kevin
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- Dan Cairns @ Kevin Chandler on Apr 5, 2019 3:01 PM
  Mark Correct
  Correct Answer
  I did look and wasn't finding someone else having this exact same issue, do you mind giving me an example?
  Should I change the concentric relationship to a coradial one, or delete the concentric relationship entirely and create the coradial one from scratch? This will be interesting because the part was created with a revolve and not a circle + extrusion.
  
  Thanks
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  - Kevin Chandler @ Dan Cairns on Apr 5, 2019 3:48 PM
    Mark Correct
    Correct Answer
    Dan Cairns wrote:
    
    I did look and wasn't finding someone else having this exact same issue, do you mind giving me an example?
    Should I change the concentric relationship to a coradial one, or delete the concentric relationship entirely and create the coradial one from scratch? This will be interesting because the part was created with a revolve and not a circle + extrusion.
    
    Thanks
    Hello,
    
    The search was just a reminder because there have been many gear posts and you may find search usual for other issues.
    
    That typed, Delete the concentric at the OD and add a coradial with the tooth's arc and the OD's edge.
    
    That should suffice (I believe).
    
    Kevin
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    - Dan Cairns @ Kevin Chandler on Apr 5, 2019 3:55 PM
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      Correct Answer
      Yup, I have tried that and doing so seems to over define the sketch. There's a fixed relation at the bottom of the tooth but if I don't keep that it seemingly makes things worse.
      Like • Show 1 Like1
      Actions
      - Kevin Chandler @ Dan Cairns on Apr 5, 2019 4:09 PM
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        Correct Answer
        Dan Cairns wrote:
        
        Yup, I have tried that and doing so seems to over define the sketch. There's a fixed relation at the bottom of the tooth but if I don't keep that it seemingly makes things worse.
        Fix is generally a bad idea unless it's absolutely unavoidable (and it usually is. I see Fix as more of an indication that I got some more thinkin' to do).
        Delete the Fix relation and try placing a dimension from the root to the midpoint of the arc (right click it and select midpoint) instead.
        
        Your Plane3 has gone into the red, too.
        I don't know what went missing, but these selections should remain after model edits:
        After this, your M5 is still narfed up.
        Like me, this dim appears to have lost its marbles somewhere.
        But it's not needed, because you've correctly modeled at the origin and about the default planes (YEAH!!!), so delete the dim and the current point and add a new point at the origin.
        
        Kevin
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        Dan Cairns @ Kevin Chandler on Apr 8, 2019 12:38 PM
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        Thank you!
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M. B. Apr 5, 2019 4:24 PM
Mark Correct
Correct Answer
Here is a method that does what you asked for but is probably not what you want if you want accurate gear teeth.

Assuming that you can't make changes to the tooth sketch, this will allow you to use the original sketch without modifying the tooth profile. I've added a derived sketch, 3 equations, and a few other minor sketch changes. Also added the R22.5 & R15 configurations.

Keep in mind that all this does is get you moving along with an inaccurate but pictorially correct gear. If you want an accurate tooth profile for different OD sizes, you will need to make significant additional modifications to the original sketch.
Attachments
- 07-01-0232.SLDPRT.zip571.5 KB
Like • Show 1 Like1
Actions
Dennis Dohogne Apr 8, 2019 7:23 AM
Mark Correct
Correct Answer
Dan,
That model you are working with apparently was not made with a good plan toward changes. Here is a good parametric gear model I made. Just edit the Design Table and change the values in the three green columns.
Attachments
- Involute Gear, Metric, DesignTable 2016.SLDPRT.zip432.6 KB
Like • Show 0 Likes0
Actions

Changing location of gear tooth with gear's overall dimension

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