It's turned out to be harder than I thought. my method above doesn't appear to work, probably because the swept cut would be self-intersecting. So I ended up getting it to work by doing two swept cuts, each using half of the groove profile. I have attached the model made in SW2014.
Sorry I won't be able to attach screen shots but I'll try to describe it the best I can.
I created a boss-extrude for the center shaft first. Then created a helix which wrapped around it 3 times, using the height and revolutions option. I then created two sketches one at the start and one at the end of the helix. These are going to be used for a loft feature, create a rectangle and dimension it for the height of your "threads", note you may need to have the end where it meets the shaft actually be dimensioned to interfere with that shaft or you may get a "zero thickness" error. For the end sketch, since the thread tapers down create a very thin rectangle, lofts seem to work best when the profiles are the same, or have the same number of vertices.
When you create the loft, use the two sketches as the profiles, but then use the centerline option and use the helix as the center line. The loft will then taper down as it goes from one profile to the next. Then just use a fillet on both sides of the thread and do an extrude cut or two to clean up your ends depending on how you have them, or how they ended up because of the helix.
many thanks for your effort to support, but actually i cannot imagine the process in 3d form. i'm sorry
It is hard to tell from the image but this solution assumes that the width of the groove is constant. I would start with a cylinder of the OD size, then make a variable pitch helix to reduce the pitch as it goes along the shaft. Then sketch the groove at one end of the helix and do a swept cut. I'll try to do an example.
I HOPE THAT THERE IS AN ANOTHER METHOD ALSO.
An simple way to use is to draw an helix with an variable pitch with an single section cut sweep method.
perfect model, but i need to understand the design intent because the next step is to make this shaft parametric, many thanks for the model
i need to understand the parameters, specially in helix curves.
why you selected this values ?depending on what ?
I'll step through all of the parameters and try to explain how you would choose them.
Sketch1 circle diameter .400 = OD of the part.
Boss-Extrude1 distance 3.000 = length of the part.
Sketch3 distance .250 = inner diameter inside the groove. You could also dimension between the inner line and the construction line to define the depth of the groove.
Sketch3 distance .750 = axial length of the groove.
Sketch3 R.200 = Radius of the side of the groove, I just guessed something that looked similar to your picture.
Note: I extended the profile out past the OD of the part just to make sure the sweep didn't leave behind any thin body around the outside.
Sketch4 = I just converted entities of half the profile.
Sketch2 = I just converted the OD of the part.
Helix/Spiral1 P1 (1in) = This is the pitch of the spiral at the beginning. You could determine this value by measuring the axial length of the groove plus the OD section at the beginning of the part (hopefully the picture explains what I mean).
Helix/Spiral1 H2 (3.75in) = I made this equal to the height of the part plus the groove length, to make sure the groove cut went all the way down the entire part.
Helix/Spiral1 P2 (.65in) = This is the pitch at the end of the spiral. I just fiddled with this number until the part looked right. I'm not really sure how you would determine what this needs to be exactly.
Plane2 is located at the midpoint of the groove profile.
Sketch8 is converted entities of the other half of the profile.
Helix/Spiral2 uses the exact same parameters as the first helix.
thanks for the clarification but unfortunately i couldn't apply this procedure on the part i have
i attached the source and the one that i model it. if you could help to model the imported body i would be grateful.
Microsoft OneDrive - Access files anywhere. Create docs with free Office Online.
Unfortunately I have SW2014 so I can't open your files. Can you attach a parasolid or step file of the imported part?
ok, this is the parasolid file ( the original one ) and the my model with version 2014
I can't get it to work. I tried breaking the cut up into 3 different sections to enable using a smaller pitch at the end of the helix, but I can't get the third cut to succeed. I keep getting "Operation failed due to geometric condition". Sorry I can't be of more help.
this is exactly what i thought at the beginning but when proceed in modeling i got the difficulty
Retrieving data ...