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Helical Gears - Utility now working for external gears.

bolsover

Senior Member
I've been playing about with a few ideas for generating helical gears.
My initial idea was to sketch the gear profile (using my involute gear generator utility) and then extrude a helical boss. This does not work because the generated solid would be self intersecting which Alibre does not allow.
The second idea was to take a single tooth sketch, extrude a helical boss and then circular pattern this for the number of teeth, This works OK but I'm still puzzled about how to set the correct pitch for the helical boss.
My question is this: Is there a 'standard' pitch or helix angle for 'standard' helical gears?
I've read several on-line articles but can't find and reference to standards.

Any suggestions?
 

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albie0803

Alibre Super User
No. Helical gears allow for smooth running but can also be tweaked to fit the box. Increasing the helix angle will also grow the Outside Diameter . I have drawings where the helix angles are defined down to minutes and seconds.

eg 11T 2.5M 20°PA
helix° - OD
8° - 32.770
10° - 32.924
12° - 33.114
14° - 33.342

Not big values, but important differences when it comes to gears, particularly high speed ones
 

bolsover

Senior Member
@albie0803
Helix angle: I thought that might be the answer.
I'd not taken the change in the transverse module into account - Thankfully a simple formula.
If my understanding is correct...

Transverse module = Normal module / Cos Helix angle
P.C.D = Transverse module * Teeth
O.D. = P.C.D + 2 * Addendum

I'd really like to automate the whole process but limitations in the Alibre API prevent that at present.

I already have a routine for straight cut gears but modelling a helical gear requires the helical boss and circular pattern functions neither of which are exposed in the V25 or earlier API.

I have submitted an enhancement request.

David
 

idslk

Alibre Super User
Hello David,

only for my curiosity - what will you do with those designed parts? Will you manufacture them? For what purpose?

Thank you for an answer in advance :)

Regards
Stefan
 

bolsover

Senior Member
Hello David,

only for my curiosity - what will you do with those designed parts? Will you manufacture them? For what purpose?

Thank you for an answer in advance :)

Regards
Stefan
@idslk
I aim to 3D print the gears and want to use helical gears in order to improve power handling. I may even go to dual helical in an effort to eliminate end thrust. Herringbone gears look interesting but I'm concerned about debris getting trapped at the root.
I've not got into the ratios I need yet - but nothing extreme.
David
 

albie0803

Alibre Super User
I already have a routine for straight cut gears but modelling a helical gear requires the helical boss and circular pattern functions neither of which are exposed in the V25 or earlier API.

I have submitted an enhancement request.
I also want the same functions and have also asked. Maybe maybe!

Helical Gear shapes
The helix angle is calculated at the pcd
Find Y for a line at helix angle from vertical where X = the circumference of the pcd
Draw a tooth shape above or below the gear blank
Do a helical cut/extrude for 1 rev over distance Y using the NORMAL feature. This is CRITICAL for correct tooth shape
Circular patten resulting feature.
 

albie0803

Alibre Super User
Afaik, They don't actually need teeth meeting at the root to work.
They don't. They are often machined with a groove in them for ease of manufacture.
Herringbones are also not true helical gears, they are a class to themselves and basically obsolete.
More common these days are left and right hand gear sets working in pairs.
1657861802123.png
 
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bolsover

Senior Member
I also want the same functions and have also asked. Maybe maybe!

Helical Gear shapes
The helix angle is calculated at the pcd
Find Y for a line at helix angle from vertical where X = the circumference of the pcd
Draw a tooth shape above or below the gear blank
Do a helical cut/extrude for 1 rev over distance Y using the NORMAL feature. This is CRITICAL for correct tooth shape
Circular patten resulting feature.
I'm working out the basics in excel - then checking in Alibre
So far..
Example gear:
Normal Module 1
Normal Pressure Angle 20 deg
Helix Angle 15 deg
Teeth 17

Calculations:.. Now with corrected value of Pi!
Normal Pitch = Normal Module * Pi = 1 * 3.141593 = 3.141593
Transverse Module = Normal Module / Cos(Helix Angle) = 1 / Cos(15) = 1.035276
Transverse PCD = Transverse Module * Teeth = 1.035276 * 17 = 17.59970
Transverse Pitch = Transverse PCD * Pi / Teeth = 17.59970 * 3.141593/ 17 = 3.252416
Axial Pitch = Transverse Pitch / Tan(Helix Angle) = 3.252416 / Tan(15) = 12.13818
Helix Pitch Length = Axial Pitch * Teeth = 12.13818 * 17 = 206.3491

Helix Pitch Length is your Y value

I now need to modify my existing C# code to generate a single tooth profile of the corrected (transverse) module size from which I can helical extrude along the required distance.

David
 
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albie0803

Alibre Super User
I now need to modify my existing C# code to generate a single tooth profile of the corrected (transverse) module size from which I can helical extrude along the required distance.

The logic below is just from my observations of the gearcutting process
A 1M hob is used to create a spur gear.
The same 1M hob is used to create a helical gear.
The tooth shape at the normal to the helix angle is still a correct 1M 20°PA shape, so the helical extrude along the normal will be correct. See here
If you use a Transverse module shape, you would need to extrude along the parallel
transverse.gif

I guess both would be right, but I would think it's much easier to use the involute shape you already have.

Herringbone gears are cut with a rack cutter as shown here and are not cut along the normal, but would use the parallel method.

1657964067986.png
Helical on the Advanced tab
 

bolsover

Senior Member
The logic below is just from my observations of the gearcutting process
A 1M hob is used to create a spur gear.
The same 1M hob is used to create a helical gear.
The tooth shape at the normal to the helix angle is still a correct 1M 20°PA shape, so the helical extrude along the normal will be correct. See here
If you use a Transverse module shape, you would need to extrude along the parallel
transverse.gif

I guess both would be right, but I would think it's much easier to use the involute shape you already have.

Herringbone gears are cut with a rack cutter as shown here and are not cut along the normal, but would use the parallel method.

View attachment 36532
Helical on the Advanced tab

@albie0803
Thanks for the advice - I need every bit I can get!
Calculating the Transverse module shape from the normal module is reasonably simple and extruding along the parallel certainly appears to be the easier option.
The tricky part (to my mind) is deciding what 'adjustments' to make to the profile.
I've found a few good sources of information such as "Calculation of involute gears" and "Geometry / Helical Gears". Together these seem to provide most of the math needed but what are the 'correct' figures for 'profile shift', 'tip shortening' and 'tip radius'. I suspect the answer lies in the specific standard being followed: JIS, ANSI, DIN etc. More reading needed!!

I have an idea as to how I might be able to create parts complete with the necessary helical boss and circular pattern features...

If I save a file with a <Tooth> sketch and the Helical Boss and Circular Pattern features it MIGHT be possible to programmatically open this file, and amend the Sketch, Helical Boss and Circular pattern features before regenerating.

I'm already creating sketches so I think a small step to modify one.
With the file open it should the simple to iterate though the part features to find the AD_HELICAL_FEATURE and AD_PATTERN_FEATURE. I should then be able to amend the Hight and Pitch of the Helical Boss and instances of the circular pattern.

Lot's of ifs and maybes but worth a try...

David
 

bolsover

Senior Member
I did some more hunting; changing an existing file might be simpler than I initially thought.
I just need to change the value of a couple of parameters IADParameter exposes the property Value for get and set. Just need to find the right parameters and edit.
Now to try out..
 

bolsover

Senior Member
Making progress...
In my quest to produce accurate models of helical gears I realised that I first needed to properly understand the geometry of standard involute spur gears.
After much reading and some experimenting with the formulae, I 'think' I now have most of the math of profile shifted spur gear covered.
I've put it all together in a user control:

Screenshot 2022-08-14 152635.png

A lot of the complexity in profile shifted gears stems from the need to calculate the various dimensions as a pair of gears.
I'm trying to keep the user inputs down to the bare minimum:
Module size, Pressure angle, teeth per gear.
It becomes much more complicated when the operating centre distance is introduced since this requires recalculation of the increment factor and total profile shift.
Distribution of the total profile shift is tricky because there is no single rule governing how this is done - so I introduced a slider control so the user can make his own choice.
I aim to provide some indication of when (if) the shift applied eliminates the need for undercutting but have not done that yet.
I have already introduced a factor for circumferential backlash but would like to also add a factor for radial backlash.

There is a long way to go.. but I have generated a couple of test gears in Alibre - look OK so far.
For the Alibre part of the task, I have set up a 'template' file with a simple sketch, an extrusion and a circular pattern.
When building the gear from the application, the template file opened, the existing sketch is opened and modified to show just a single tooth. The sketch is then closed and the circular pattern modified to show the correct number of teeth before regenerating the whole this to show the completed gear.

I'd welcome comments!

David
 

bolsover

Senior Member
I'm not quite ready for a release of a tool that can generate helical gears yet but I have done quite a bit of work with that aim in mind.

So, I've just uploaded a tool that can generate standard and profile adjusted spur gears.

I've tried to keep it as simple as possible but I should note that profile shifting is complex!

I'm fully aware of a couple of deficiencies; in particular, it does not adjust the generated profile for possible undercutting so I don't recommend its use for gears having fewer than 17 teeth although you might just about get away with it if appropriate backlash is applied.

Standard gears are a breeze - just enter module, pressure angle and teeth required, set the operating centre distance and build the gears.
Note that the operating centre distance is NOT automatically set but is red if not is not the same as the standard centre distance.

Profile shifting is a matter of setting the required operating centre distance and adjusting the distribution of profile shift if needed.
Note that contact ratio should be maintained above 1.2 - or the gear will probably not work effectively.

The gear models are generated from template files (V25). This tool will NOT work with earlier version.
Once a gear has been generated, you'll need to use save-as to put the file where needed by default it is in the user temp directory.

The setup file is available together with the source code.

https://github.com/bolsover/UtilitiesForAlibre/releases/tag/V1.1.0.0

All comments welcome

David

Gear Generator.png
 
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