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How to create screw-thread
jan_willem
Member Posts: 5 ✭✭
Hello,
I would like to learn how I can draw screw-threads in my sketch. Metric, for example M8. I can not find whether it is possible and if so how. The only thing i can find is to create a helix…
Who can help me?
Best regard,
Jan-Willem
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Best Answers
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Optionsandrew_troup
Member, Mentor Posts: 1,584 ✭✭✭✭✭
The info you need is in this recent thread
https://forum.onshape.com/discussion/comment/4867/#Comment_4867
paying particular attention to the comments from @Coleman and @LouGallo5 -
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coleman
OS Professional Posts: 244 ✭✭✭
1) Create feature (major OD of screw, bolt, lead-screw, etc.)
2) Create helix on previous feature. Select number of turns or pitch for helix
3) Create a plane to sketch the thread profile (cutting tool) on.- Select plane icon
- Select "curve point" from dropdown
- Select vertex of Helix (defining start point) TIP: hide part in parts tree to easily select the vertex.
- Select body of Helix (defining normal of the plane)
5) Create a sweep. Use the thread profile sketch as the "faces, sketches and regions to sweep" & the helix as the "sweep profile." To simulate cutting thread use the remove command.
Troubleshooting if you get an error on the sweep command:- Make sure your thread profile is a closed sketch
- Make sure your thread profile can actually wrap (sweep) around the helix path without cutting into itself on adjacent passes. For example: if you use a 60 degree V thread with a pitch of .020in and the thread profile sketch has a .125in width it will break because the tool is too big to cut a small feature.
- Start with the smallest thread profile (cutting tool) you can use and still get the desired thread. I usually create a smaller thread profile sketch and then execute the sweep command. After I get the preliminary sweep and profile, I edit the thread profile sketch and increase the size of the thread profile in small increments, making sure the sweep doesn't break as I increase the size of the profile.
- To thread to the tip of a screw: 2 helix profiles are used. 1 for straight shaft, other for tapered tip of screw. Create both helix profiles. Hide the part in the parts tree and you can still see the two helix profiles. Adjust the start point angle of one helix until the vertices of the two helixes mate up perfectly. This is a little trial and error. Keep adjusting until they mate. ( I am confident that in future updates this step won't be necessary.) Execute one sweep command and select both helixes as the path.
- To clean up where thread stops and starts: I usually select the face (where thread stopped) and create a sketch. Project the edges ("use" command) onto the active sketch plane and extrude remove. This simulates essentially (ok almost) what a lathe will do when the tool rapids off the part while cutting threads. In the future OS will provide the ability to extend helixes beyond the feature they are slaved to, which will allow for a lead in and lead out.
6 -
Optionsr_paul
Member Posts: 22 ✭✭
Jan-Willem
The link below may give you a good idea as to how to model a screw and nuts also.
You will notice I have only used one helix for each component allowing the chamfers to show a correct start to the thread.
Coleman has indicated, to get the threads in both the screw and nut to align I needed to watch the start points. This is not too difficult if when using the Helix command you will see the Helix start at a particular point on you cylinder of choice (solid or surface). Adjusting the start point in 90 increments will probably give you the correct result.
If the thread (solid Helix) end needs a run-out I Extrude the end face of the solid>Helix approximately the radius of the threaded shaft. That will normally give a good (visual) lead-out and means you only have the one Boolean (Subtract/Remove) to do.
https://cad.onshape.com/documents/7bf6e574fc944b11b3cf6d5d/w/bce9145f8201438f99283a86/e/082d8b969c904c5aaca1bd2f
5
Answers
https://forum.onshape.com/discussion/comment/4867/#Comment_4867
paying particular attention to the comments from @Coleman and @LouGallo
2) Create helix on previous feature. Select number of turns or pitch for helix
3) Create a plane to sketch the thread profile (cutting tool) on.
- Select plane icon
- Select "curve point" from dropdown
- Select vertex of Helix (defining start point) TIP: hide part in parts tree to easily select the vertex.
- Select body of Helix (defining normal of the plane)
4) Using the plane you just created, sketch the thread profile (V-thread, Acme, Buttress, circle, etc.). Make sure it is a closed sketch profile. Set the thread depth (minor OD) with dimension from centerline of major OD. I usually sketch a construction centerline and dimension from here.5) Create a sweep. Use the thread profile sketch as the "faces, sketches and regions to sweep" & the helix as the "sweep profile." To simulate cutting thread use the remove command.
Troubleshooting if you get an error on the sweep command:
- Make sure your thread profile is a closed sketch
- Make sure your thread profile can actually wrap (sweep) around the helix path without cutting into itself on adjacent passes. For example: if you use a 60 degree V thread with a pitch of .020in and the thread profile sketch has a .125in width it will break because the tool is too big to cut a small feature.
Tips:- Start with the smallest thread profile (cutting tool) you can use and still get the desired thread. I usually create a smaller thread profile sketch and then execute the sweep command. After I get the preliminary sweep and profile, I edit the thread profile sketch and increase the size of the thread profile in small increments, making sure the sweep doesn't break as I increase the size of the profile.
- To thread to the tip of a screw: 2 helix profiles are used. 1 for straight shaft, other for tapered tip of screw. Create both helix profiles. Hide the part in the parts tree and you can still see the two helix profiles. Adjust the start point angle of one helix until the vertices of the two helixes mate up perfectly. This is a little trial and error. Keep adjusting until they mate. ( I am confident that in future updates this step won't be necessary.) Execute one sweep command and select both helixes as the path.
- To clean up where thread stops and starts: I usually select the face (where thread stopped) and create a sketch. Project the edges ("use" command) onto the active sketch plane and extrude remove. This simulates essentially (ok almost) what a lathe will do when the tool rapids off the part while cutting threads. In the future OS will provide the ability to extend helixes beyond the feature they are slaved to, which will allow for a lead in and lead out.
Good luck!Jan-Willem
The link below may give you a good idea as to how to model a screw and nuts also.
You will notice I have only used one helix for each component allowing the chamfers to show a correct start to the thread.
Coleman has indicated, to get the threads in both the screw and nut to align I needed to watch the start points. This is not too difficult if when using the Helix command you will see the Helix start at a particular point on you cylinder of choice (solid or surface). Adjusting the start point in 90 increments will probably give you the correct result.
If the thread (solid Helix) end needs a run-out I Extrude the end face of the solid>Helix approximately the radius of the threaded shaft. That will normally give a good (visual) lead-out and means you only have the one Boolean (Subtract/Remove) to do.
https://cad.onshape.com/documents/7bf6e574fc944b11b3cf6d5d/w/bce9145f8201438f99283a86/e/082d8b969c904c5aaca1bd2f
Regards,
Jan-Willem