helical gear tooth profile, how do I get the right helix angle with coil tool?

[Anonymous]

I have generated a gear set using inventor. Now I would like to 3d print the gears. I have uesd the export tooth shape to get the true tooth profile. now I am attempting to use the coil feature to generate the helical tooth. The problem im running into is in the coil tool I can only give it a Revolution and height dimension. The hight is the width of the gear, but I am having a problem converting the helix angle to the "Revolution" perameter. I have read other posts and they say that it is Helix angle / 360. I have tried that and then compared it to the original gear generated by inventor and it is not even close. I need to do this on in internal gear and match it to an external gear. I ahve attached the generated gears i'm working with.

Thanks for the help in advance! I really apreciate it!

Andrew

[Anonymous]

So I have learned a little more trying to figure this out. In other examples people have been using the coil feature with the revolution and height setting. But what I have noticed is if you enter a number for revolution say thats close to the helix you want ( I have not figured out how to coil the correct helix angle yet) and then you change the height, it changes the helix angle. So I belive the correct method is to use the Pitch and height setting. Now I need to figure out how to calculate pitch based off of a helix angle. When you use pitch and height, then change the height it will just continue the same angle without distorting it.

If anyone want's to chime in and help me out it would be greatly appreciated! Thanks!

Andrew

[tkahle]

Although not  an expert, I recently used this method and it worked very well.

1) Design the gears using the design accelerator.

2) Export the tooth profiles.

3) Create a Coil feature

a) Coil Shape

  i) Select the tooth profile

  ii) Select Z axis

  iii) Choose "cut"

  iv) Choose desired rotation

b) Coil Size

  i) Type = Pitch and Revolution

  ii) Pitch = PitchDiameter * PI  / tan(HelixAngle)

  iii) Revolution = FaceWidth * tan(HelixAngle) / ( PitchDiameter * PI )

4) Array the coil feature.

[renatocalvinisti]

This seems to do the trick. Do you have any mathematical break through of the formulas? or a procedure of some kind on how to reach these formulas. 

Thanks!

[tkahle]

I do not. Sorry.

[johnsonshiue]

Hi! This is a very interesting discussion. If I understood the requirement correctly, the correct cut has to be done via sweeping a volume (like how it would be cut in real world). Inventor 2019 does have the ability to create smooth variable-pitch and variable-radius helical curve. But, Inventor 2019 is not yet able to sweep a volume. We are working on a robust solution which will allow users to pick a volume as a profile to sweep along various paths. If you are interested, please sign up Inventor Beta program (https://bit.ly/InventorBeta).

Many thanks!

[graemev]

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@johnsonshiue wrote:

Hi! This is a very interesting discussion. If I understood the requirement correctly, the correct cut has to be done via sweeping a volume...

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I don't believe this is the case. Standard helical gears still need an involute tooth form as described upon the end face of the gear. It's the same as a straight cut gear, just twisted.

Think of it like a stack of very thin slices with each slice rotated slightly from the adjacent slice - a stack of coins, if you will. The basic profile remains the same, but the completed stack is helical.

[johnsonshiue]

Hi! In the end, the gear has to be machined, right? Or, are you printing the gear? If the gear has to be machined, it will require sweeping a volume to accurately represent the cut. Traditional 2D profile cut simply does not cut it.

Many thanks!

[graemev]

Don't quote me on it, but to my understanding the gear cutter profiles are manufactured to take this into consideration. The cutter's line of action is set at the pitch angle and the milling proceeds along the gear's axis while the gear is rotated in a coordinated fashion.