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bolsover

Senior Member
I'm working on an update to my gear generator and need some help with the geometry calculations..

I want to add a radius to the gear tooth tip. This needs to be mathematically correct and the location can not be determined by sketch construction.

Generally, the radius at the tooth tip where the Addendum (Tip) circle meets the involute curve of the tooth flank is 0.25Module.

The screen grab below illustrates the problem for a Module 1, 18 Tooth gear.

The circle at centre A is the full circle of the tip radius. This circle needs to meet the Addendum Circle at Point B and the involute of the tooth flank at point C.

What is known..
Diameter of the Addendum Circle - in the case below 20mm
The Point A has to be located on a circle diameter 19.5 in order for the tip radius to be tangent to the Addendum diameter.
Point C is at the tangent intersect of involute curve of tooth flank and tip radius circle.
Dimension A-C = A-D = 0.25Module
Coordinate (X,Y) of Point E where the involute meets the addendum is known.
Coordinate Point D (mid point of tooth tip) is known.
Gear centre is always at coordinate 0,0.

What I need to calculate..
Locations of points A, B and C.

TipRadius.png

Screen grab is taken from the attached part.

David
 

Attachments

  • TipRadius.AD_PRT
    287 KB · Views: 7

DavidJ

Administrator
Staff member
David, forgive me if I'm asking stupid questions...

Do you mean 0.25 x Module for size of radius (in mm)? - so 0.25mm in this example.

When you say ' location can not be determined by sketch construction' - do you mean this is impossible, or that it isn't an option for your utility because it would require manual intervention? I was able to apply tangent sketch constraint to the circle in your sketch and the spline representing the involute.

Not sure I can necessarily help with the maths, I just wanted to be clear on the question.

Can you simply apply 3D fillet to the edges of the extruded tooth?
 
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simonb65

Alibre Super User
Can you simply apply 3D fillet to the edges of the extruded tooth?
Not sure if programmatically (with the API) you can determine the edge that the fillet(s) need to be placed on once the sketch is extruded as the edge names (required by the fillet function), etc will all be internally generated by the Extrude function and won't be distinguishable from the internal corners at the base of the tooth! That task would be made easier if the edge entity had an 'internal' or 'external' property.

Not sure how you'd calculate that based on the fact they all need to be derived from points on arcs .. my maths certainly isn't up to that without plenty of coffee and hours of head scratching.
 

DavidJ

Administrator
Staff member
Surely if a 'template tooth sector' is used the edge IDs that need to be filleted will always have same ID, so can be 'hard coded' - or perhaps I've mis-understood.
 
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NateLiquidGravity

Alibre Super User
I'm working on an update to my gear generator and need some help with the geometry calculations..

I want to add a radius to the gear tooth tip. This needs to be mathematically correct and the location can not be determined by sketch construction.

Generally, the radius at the tooth tip where the Addendum (Tip) circle meets the involute curve of the tooth flank is 0.25Module.

The screen grab below illustrates the problem for a Module 1, 18 Tooth gear.

The circle at centre A is the full circle of the tip radius. This circle needs to meet the Addendum Circle at Point B and the involute of the tooth flank at point C.

What is known..
Diameter of the Addendum Circle - in the case below 20mm
The Point A has to be located on a circle diameter 19.5 in order for the tip radius to be tangent to the Addendum diameter.
Point C is at the tangent intersect of involute curve of tooth flank and tip radius circle.
Dimension A-C = A-D = 0.25Module
Coordinate (X,Y) of Point E where the involute meets the addendum is known.
Coordinate Point D (mid point of tooth tip) is known.
Gear centre is always at coordinate 0,0.

What I need to calculate..
Locations of points A, B and C.

View attachment 37158

Screen grab is taken from the attached part.

David
I've made a script that calculates and adds a radius to any two non-parallel lines given the two lines and the radius - which is a function Alibre should include out-of-the-box - but you can have it if it helps.
 

simonb65

Alibre Super User
I've made a script that calculates and adds a radius to any two non-parallel lines given the two lines and the radius
The two 'lines' here are both arcs/radii (tooth face and gear outer diameter), so not sure if your calculation would help here.
 

oldfox

Alibre Super User
David,
I can't use your .prt because I'm still on V24. I believe there is a way you can construct the tooth tip. I just need verification of all of the lines and circles.
I think that Vector "B" is from the center of the gear through the center of the tooth? I think the red Arc is the tooth face? And the orange circle is the full circle of the tip arc?
If that is correct I can probably construct enough for you to see how I would do it. Can you enable "Sketch dimensions" and delete most of the unnecessary stuff and re-post it as a JPEG?
 

bolsover

Senior Member
@DavidJ
Yes 0.25 * Module.
Location - I have an Add-On utility that generates the existing sketch for any module, tooth count, pressure angle and helix angle as required.
Because this is part of an Add-On, the sketch figures need to be added by calls to the relevant API methods. For the tip radius, I'll almost certainly be making a call to IADSketchFigures.AddCircularArcByCenterStartEnd... So all the parameters need to be calculated.

The existing utility is available here if you want to try out. https://github.com/bolsover/UtilitiesForAlibre/releases

@simonb65
I hadn't considered applying a fillet after extruding the tooth. That could work and is certainly easier than all the sketch calculations.:)
I'll test to find out if it can be automated. I will need to make some changes to the template part file currently used.

@NateLiqGrav
As Simon noted, the issue I have is with arcs rather than lines - but I'd be gad to have a copy in your routine anyway.

@oldfox
Sorry it's V25 only but I'll try to post a friendlier view for you soon.

I have made a little (conceptual) progress myself..
The screen grab below is just a small section of the tooth tip. I can calculate the location of a point on the involute flank where the 19.5 circle intersects. I already know the location of the point at the apex where the involute meets the addendum circle.

I have drawn a couple of construction lines: one from the intersection of 19.5 circle with involute to tooth tip and a second length 0.25 perpendicular to the first and with end at point A coincident with 19.5 circle.

This may help. if I can calculate the 19.753 dimension....

TipRadius1.png
 

simonb65

Alibre Super User
@bolsover You could use the centre points of the tooth face and centre of the gear to create 2 arcs that are there respective radius minus the fillet radius. Then find the intersecting points of those two new arcs (should able able to find a formula for that on the web) using quadratic equations. That will give you 2 possible results and you'd need to figure out which was the correct one to give you the centre of the fillet at point 'A'. Working out 'B' and 'C' would be the next problem !

Interesting problem to solve though! :)
 
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bolsover

Senior Member
David,
I can't use your .prt because I'm still on V24. I believe there is a way you can construct the tooth tip. I just need verification of all of the lines and circles.
I think that Vector "B" is from the center of the gear through the center of the tooth? I think the red Arc is the tooth face? And the orange circle is the full circle of the tip arc?
If that is correct I can probably construct enough for you to see how I would do it. Can you enable "Sketch dimensions" and delete most of the unnecessary stuff and re-post it as a JPEG?
Sorry I can't post a V24 version but vector 'D' is the centre of the gear. Red arc is indeed the tooth face. This is actually a spline having 25 control points the location of which are calculated to be on the correct involute curve..
David
 

oldfox

Alibre Super User
The trick I use is to use 2 circles, one centered on Point "B" and the other one centered on an offset of the tooth face. I believe you can find the second by using offsets.
Then use the intersection of the 2 circles which are both of tip arc diameter. Where the 2 circles intersect is the center for you tip arc, tangent to both knowns.
 

bolsover

Senior Member
@bolsover You could use the centre points of the tooth face and centre of the gear to create 2 arcs that are there respective radius minus the fillet radius. Then find the intersecting points of those two new arcs (should able able to find a formula for that on the web) using quadratic equations. That will give you 2 possible results and you'd need to figure out which was the correct one to give you the centre of the fillet at point 'A'. Working out 'B' and 'C' would be the next problem !

Interesting problem to solve though! :)
@simonb65 @oldfox
This has certainly given me a possible way forward. I just sketched this.. looks promising.
David
TipRadius2.png
 

DavidJ

Administrator
Staff member
In this adjusted version of your part, the fillet is applied to edges 18 & 21. Unless there is radical change to the template, I don't see why the edges to fillet would change, though obviously the count for the pattern would....
 

Attachments

  • TipRadius.AD_PRT
    1.7 MB · Views: 4

simonb65

Alibre Super User
I was thinking more ...

1662572504800.png

Where A is the intersection of the Dia/Tooth face minus the rad (shown by reference circles) ... it's part of the solution. At least you know the centre of the fillet arc. Just need to figure out the start and end points.

You could probably work out the points on the outer diameter and tooth face using vectors from the centres of those through point A where they intersect with the dia/tooth face OR the angles from the arc centres to point A !!!!
 

albie0803

Alibre Super User
Personally I wouldn't worry. The gear hobs and rack cutters we use here do not generate a radius on the tooth edge. We often manually put a chamfer on the top and bottom of the tooth but not along the tip edge like you are talking about.
 

Attachments

  • IMG_3199.JPG
    IMG_3199.JPG
    1.4 MB · Views: 19

NateLiquidGravity

Alibre Super User
@simonb65
I hadn't considered applying a fillet after extruding the tooth. That could work and is certainly easier than all the sketch calculations.:)
I'll test to find out if it can be automated. I will need to make some changes to the template part file currently used
That could work and be easier in this situation. You could loop through all edges.
Immediately throw out any that are parallel with the sketch (both end points on same "elevation").
Loop through the remaining edges and check if they fall on that radius distance from the gear center.
Apply a 3d fillet to those remaining edges.
 

bolsover

Senior Member
Personally I wouldn't worry. The gear hobs and rack cutters we use here do not generate a radius on the tooth edge. We often manually put a chamfer on the top and bottom of the tooth but not along the tip edge like you are talking about.
I'm really interested in modelling gears for 3D printing where a radius tip is quite natural.
Do you employ any sort of tip relief to prevent chipping of the tooth?
David
 

bolsover

Senior Member
That could work and be easier in this situation. You could loop through all edges.
Immediately throw out any that are parallel with the sketch (both end points on same "elevation").
Loop through the remaining edges and check if they fall on that radius distance from the gear center.
Apply a 3d fillet to those remaining edges.
I have found a problem trying to programmatically add fillets.
In order to add a fillet, the 3D representation of a single tooth needs to exist. This probably OK for straight cut gears where there is an API method for AddExtrudeBoss. However, it fails when considering Helical gears because there is no API method for AddHelicalBoss (I have requested an enhancement). Without the 3D representation, you can't add the fillets (at least not that I have found) and searching for the relevant features seems problematic.
The other issue is that there is no API for Circular Patterns. I overcame these issues in my code by preparing custom, pre formatted .prt files with the appropriate extrusions and patterns. All that remained was to adjust a couple of parameters after the gear tooth sketch was fully formed and regenerate all.

Frustrating that there are so many (essential?) features missing from the API. I have quite a few ideas for automated routines...

So, I'm going back to getting fully formed sketch from which the gears can be generated.

David
 

bolsover

Senior Member
I was thinking more ...

View attachment 37169

Where A is the intersection of the Dia/Tooth face minus the rad (shown by reference circles) ... it's part of the solution. At least you know the centre of the fillet arc. Just need to figure out the start and end points.

You could probably work out the points on the outer diameter and tooth face using vectors from the centres of those through point A where they intersect with the dia/tooth face OR the angles from the arc centres to point A !!!!
Hi Simon. Sorry I misunderstood your suggestion. But there is a problem anyway. The tooth face is not circular, it is involute so doesn't have a diameter in the normal sense.
However, with all the suggestions that have come forward, I think I may have a way ahead. I'll continue working at the sketch level and may need an iterative solution - but that what computers are good at!.
David
 

simonb65

Alibre Super User
The tooth face is not circular, it is involute so doesn't have a diameter in the normal sense.
Mathematically you should still be able to generate an offset (by the fillet radius) and create the involute for that, then quadratically solve that formula with the diameter formula. It does add more complexity, but as you say someone with a great understanding of the maths would know how!

Is the involute generated from a series of calculated lines then? So can you do some interpolation and approximation to get the points you need? ... or is it a spline?
 
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