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JDMather
Posts: 26,186
Registered: ‎04-20-2006
Message 11 of 18 (461 Views)

Re: Helical Gear in inventor

11-17-2011 07:23 AM in reply to: 1111111222222222222

1111111222222222222 wrote:

I done this in other way by using sweep option (Sweep a profile along a path).  


I think I would have used Coil (SWx doesn't have this command and requires you to create a 2D circle sketch to define a 3D helix path and then of course create the 3D helix path and finally Sweep).

 

Attach your file here.

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Member
tkahle
Posts: 4
Registered: ‎02-06-2013
Message 12 of 18 (370 Views)

Re: Helical Gear in inventor

02-09-2013 07:48 PM in reply to: JDMather

JDMather,

It is my understanding that gears generated by the design accelerator are rough approximations of the ideal, and that the gear tooth profiles exported from the design accelerator are precise representations.  I have used these exported profiles to create spur gears successfully.  It is important for me to have my models be accurate as they are directly used to create injection molds for manufacturing these gears.  Now I am designing a pair of helical gears.  I have a strong belief that this strategy of using the design accelerator to create the helical gears, and then exporting the tooth profile to create the accurate model is the correct way to go.  Based on your comment "I think I would have used coil", you must agree.  I am having trouble understanding how to convert the helix angle into the inputs of the coil feature.  Could you help with this?  With the correct inputs, will the resultant part be an accurate representation so that it could be used to create the mold?  Thanks for your consideration.

Member
tkahle
Posts: 4
Registered: ‎02-06-2013
Message 13 of 18 (341 Views)

Re: Helical Gear in inventor

02-11-2013 06:25 AM in reply to: tkahle

I believe I have identified the quintessential method of generating precise helical gears.

 

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.

 

That's it.  It seems to work perfectly.  Someone correct me if I'm wrong, please.

Distinguished Contributor
SKinzel
Posts: 133
Registered: ‎06-12-2007
Message 14 of 18 (324 Views)

Re: Helical Gear in inventor

02-11-2013 10:44 AM in reply to: JDMather

How do you export the tooth profiles?  The best I could come up with is to select the face of the gear and export that but when I imported that into a sketch it didn't come in as a closed profile.  I didn't see a way to "directly" export the tooth profile.

Stuart Kinzel
Inventor 2013-64bit, HP EliteBook8740w Intel Core i5CPU 2.67 GHz
8GB memory
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JDMather
Posts: 26,186
Registered: ‎04-20-2006
Message 15 of 18 (313 Views)

Re: Helical Gear in inventor

02-11-2013 11:41 AM in reply to: SKinzel

Right click on the Design Accelerator node

 

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Active Contributor
shirazbj
Posts: 46
Registered: ‎02-25-2007
Message 16 of 18 (299 Views)

Re: Helical Gear in inventor

02-11-2013 06:46 PM in reply to: stevec781

It's interesting to use coil feature.

 

But I think the profile is not perpendicular to the path.

 

So, it's just a simplify.

 

Am I right?

 

Regards,

 

Peter

Member
tkahle
Posts: 4
Registered: ‎02-06-2013
Message 17 of 18 (275 Views)

Re: Helical Gear in inventor

02-12-2013 06:02 PM in reply to: shirazbj

"But I think the profile is not perpendicular to the path."

 

That is a good point.  I wish an authoritative source would set the record straight.

Employee
alesricar
Posts: 12
Registered: ‎05-25-2006
Message 18 of 18 (87 Views)

Re: Helical Gear in inventor

04-14-2014 03:40 PM in reply to: tkahle
Late response.... but perhaps still valid.
The profile is computed as a projection to the plane so it is fine to use coil feature. The tool is designed for that.

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