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Helical Gear in inventor

22 REPLIES 22
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Message 1 of 23
1111111222222222222
13694 Views, 22 Replies

Helical Gear in inventor

Hello,

 

How to draw in Autodesk inventor Helical Gear using Flex option (this option you can find in SolidWorks) below I put link to SolidWorks where this options allow to preper gear by rotation of existing solid. Where do i find this option in Autodesk?  

 

Helical Gear

 

thank for help and advice 

22 REPLIES 22
Message 2 of 23

Gear Design Accelerator.
Start an assembly.
Save.
Click Design tab.


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Message 3 of 23

Thank for answer  Robot Mad

Can I do this the same way in Part option? I know that I can do in Assembly (Design and than choosing Spur gear option)

 

thank

bross 

Message 4 of 23

You must be in assembly.

If you only need one gear (what mechanism runs with one gear) you can delete the other.


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Message 5 of 23
stevec781
in reply to: JDMather

You can easily model a helical gear in the part environment, just use the coil feature.  Use revolution and height, that way you set the gear thickness at the same time.  If you want 15 deg just enter 15/360 in the revolution field. 

 

With a shared sketch it will take fewer steps than on the video.

 

gear.JPG

Message 6 of 23

Thanks stevec781 for answer. That's it. But I would like to know how did you do this step by step. Can you explain me or put short film? I try to do as you said but i have still problem with rotating solid.

 

Here I put drawing which i want to do.

 

Gear 

 

Thanks

bross 

Message 7 of 23


@1111111222222222222 wrote:

 I try to do as you said but i have still problem with rotating solid.

 

Thanks

bross 


Attach the file here of what you were able to complete.


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Message 8 of 23
stevec781
in reply to: JDMather

You dont need to rotate the solid, just use the coil feature.  Quick example attached.

Message 9 of 23

Attach the ipt file of what you have been able to complete on that part.


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Message 10 of 23

One more time I would like to thank you stevec781 for help and file Smiley Happy. I done this in other way by using sweep option (Sweep a profile along a path). I totally forgot about this option that I can do.

 

Thanks

bross 

Message 11 of 23


@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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Message 12 of 23
tkahle
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.

Message 13 of 23
tkahle
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.

Message 14 of 23
SKinzel
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
Windows 7 64bit
Message 15 of 23
JDMather
in reply to: SKinzel

Right click on the Design Accelerator node

 


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Message 16 of 23
shirazbj
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

Message 17 of 23
tkahle
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.

Message 18 of 23
alesricar
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.


Ales Ricar
Software Engineer
Message 19 of 23

Message 20 of 23

Hi! The precise geometry in this case needs to use Solid Sweep in 2020 and later. Profile Sweep can only approximate the geometry but it is not precise.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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