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.
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.
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.
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.
Right click on the Design Accelerator node
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