Helical Gear in inventor

[1111111222222222222]

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 

[1111111222222222222]

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 

[JDMather]

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

[JDMather]

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

[1111111222222222222]

Thank for answer 

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 

[1111111222222222222]

Thank for answer 

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 

[JDMather]

You must be in assembly.

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

[JDMather]

You must be in assembly.

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

[stevec781 · Accepted solution]

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.

[stevec781 · Accepted solution]

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.

[1111111222222222222]

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.

 

Thanks

bross 

[1111111222222222222]

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.

 

Thanks

bross 

[JDMather]

---

@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.

[JDMather]

---

@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.

[stevec781]

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

[stevec781]

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

[JDMather]

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

[JDMather]

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

[1111111222222222222]

One more time I would like to thank you stevec781 for help and file . 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 

[1111111222222222222]

One more time I would like to thank you stevec781 for help and file . 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 

[JDMather]

---

@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.

[JDMather]

---

@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.

[tkahle]

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.

[tkahle]

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.

[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.

[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.

[Anonymous]

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.

[Anonymous]

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.

[JDMather]

Right click on the Design Accelerator node

[JDMather]

Right click on the Design Accelerator node

[Anonymous]

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

[Anonymous]

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

[tkahle]

"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.

[tkahle]

"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.

[alesricar]

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.

[alesricar]

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.

[johnsonshiue]

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!

[johnsonshiue]

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!