Posted: 3/14/2026 2:16:05 PM EDT
[Last Edit: Striker][Edited]
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I won. I'm not sure exactly how though. I kept messing with the profile, path and guide rail and after many attempts the last version worked.. Another bonus is I used up a lot of filament I didn't like in the process.  I'm attempting to model the cover for a pitcher for my daughter in law. I have the bulk of it done. I'm down to creating the thread. This has to be as close to perfect as possible so the top doesn't come off when you pick the pitcher up. This is what it looks like.  |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
| Do you just need to know the pitch? As shown in your picture, measure from the top of one end of the thread to the top of the other, (easiest way to measure). That will give you inches per thread. Divide one by that number to get threads per inch. |
9 lives - 9 pellets... Coincidence?
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Originally Posted By ske714: Do you just need to know the pitch? As shown in your picture, measure from the top of one end of the thread to the top of the other, (easiest way to measure). That will give you inches per thread. Divide one by that number to get threads per inch. Not how it works with CAD. Normally, you'd create a helix the same diameter as the ID of the lid with the same pitch. Measure pitch of the thread by going either crest to crest or root to root. It's not an exact science here, it's a single turn thread. Then figure out the rough thread height and shape and model it according, and then pierce the helix you made with the profile sketch. Then just sweep. Boom, done. Fusion it's a bit wonkier, admittedly. Definitely the least easy of the big three to model in. Usually most people use the "coil" command under the create menu. I'll see if I can get a quick draft drawn up and I can upload it to the discord if you're on there. |
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Originally Posted By -Obsessed-: Not how it works with CAD. Normally, you'd create a helix the same diameter as the ID of the lid with the same pitch. Measure pitch of the thread by going either crest to crest or root to root. It's not an exact science here, it's a single turn thread. Then figure out the rough thread height and shape and model it according, and then pierce the helix you made with the profile sketch. Then just sweep. Boom, done. Fusion it's a bit wonkier, admittedly. Definitely the least easy of the big three to model in. Usually most people use the "coil" command under the create menu. I'll see if I can get a quick draft drawn up and I can upload it to the discord if you're on there. I think I'm in the discord group..
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To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By Striker: I was tracking what you were saying until create a helix.. I think I'm in the discord group.. OnShape and Solidworks both have construction geometry known as a Helix. It's basically a thread sweep path. However, there is no such feature in Fusion so you have to have a bastardized solution. The common "solution" is you use a triangular cross sectioned Coil (which is a helix body basically) that you use the outer tip of the triangle as a guide path and the inner face as a guide surface, and then you draw your actual profile on the lid's cross section, and then, you sweep, using the coil as a reference. It's a PITA as I said, but it works. Here is an example, using a circular profile (not a full semicircle, usually threads are slightly less than that) so I have it such that the tangent of the circle forms a 60º angle with the lid's top (aka print bed). This ensures printability. Of course, this is just a bullshit example and you can make it whatever you want.  First, create an offset plane (just makes the coil a bit cleaner as it's not so far removed from the actual profile. This is technically optional, you could use the XY plane. Attached File Next, create a Coil. The diameter is not important, but I like to get it sufficiently close to the actual profile. Make the pitch/revolutions match what you want your thread to be. Make the profile small enough that it's less than the actual cross section (so the profile doesn't intersect itself). Attached File Then, on the YZ or XZ plane (wherever the coil starts) draw your actual thread profile: Attached File Then sweep. The profile is is the cross section of the profile. Path is the point of the triangle. Guide curve is the back face of the coil. Attached File Then you should get something like this after you remove the coil and round off the sweep profile ends: Attached File |
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Originally Posted By Blob: Is it a multi start thread? Very common on lids and caps. Tks Obsessed...I'll give it a go. |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By -Obsessed-: Not how it works with CAD. Normally, you'd create a helix the same diameter as the ID of the lid with the same pitch. Measure pitch of the thread by going either crest to crest or root to root. It's not an exact science here, it's a single turn thread. Then figure out the rough thread height and shape and model it according, and then pierce the helix you made with the profile sketch. Then just sweep. Boom, done. Fusion it's a bit wonkier, admittedly. Definitely the least easy of the big three to model in. Usually most people use the "coil" command under the create menu. I'll see if I can get a quick draft drawn up and I can upload it to the discord if you're on there. There is a tool in SW that will do the helix and 2D profile for you. Just make the surface, select the surface and if your thread is in there just select positive or negative extrusion. I have not yet had to do one in fusion. |
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Originally Posted By Deerhurst: There is a tool in SW that will do the helix and 2D profile for you. Just make the surface, select the surface and if your thread is in there just select positive or negative extrusion. I have not yet had to do one in fusion. Built in profiles are usually no good for 3D printing as the clearances aren't sufficient. Easy enough to cut your own. Well, besides F360. Still not bad, but it's not intuitive. SW and OS definitely win on thread cutting. I have an Excel worksheet I made that I can plug in relevant details of the thread profile I want to make and it calculates everything for me. Very handy. Attached File |
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Originally Posted By -Obsessed-: Built in profiles are usually no good for 3D printing as the clearances aren't sufficient. Easy enough to cut your own. Well, besides F360. Still not bad, but it's not intuitive. SW and OS definitely win on thread cutting. I have an Excel worksheet I made that I can plug in relevant details of the thread profile I want to make and it calculates everything for me. Very handy. https://www.ar15.com/media/mediaFiles/467079/threadcalc_jpg-3729846.JPG If you wanted, you can edit Fusion's thread data .xml file or even create your own for custom vee-threads. Attached File |
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Originally Posted By -Obsessed-: Built in profiles are usually no good for 3D printing as the clearances aren't sufficient. Easy enough to cut your own. Well, besides F360. Still not bad, but it's not intuitive. SW and OS definitely win on thread cutting. I have an Excel worksheet I made that I can plug in relevant details of the thread profile I want to make and it calculates everything for me. Very handy. https://www.ar15.com/media/mediaFiles/467079/threadcalc_jpg-3729846.JPG Depends on the thread. I can do 1/2-28 with the right machine. Generally resin but I have gotten close enough for a cleanup with a tap on a FDM. The thread on that lid is pretty coarse. Drawing threads the "old fashioned" way is effective. I've done it for custom threads such as M18x24TPI when designing a HUB adapter for a DPM. I haven't done much with fusion lately with threads but I found it seems to lack many very popular and very common threads. Very infuriating when trying to make simple things so I generally just do the tap drill hole and call out the thread in the drawing (another extremely unpolished section on F360). |
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Originally Posted By Deerhurst: Depends on the thread. I can do 1/2-28 with the right machine. Generally resin but I have gotten close enough for a cleanup with a tap on a FDM. The thread on that lid is pretty coarse. Drawing threads the "old fashioned" way is effective. I've done it for custom threads such as M18x24TPI when designing a HUB adapter for a DPM. I haven't done much with fusion lately with threads but I found it seems to lack many very popular and very common threads. Very infuriating when trying to make simple things so I generally just do the tap drill hole and call out the thread in the drawing (another extremely unpolished section on F360). Fusion's included thread library is huge. Way larger than the standard thread library that came with my copy of solidworks. Fusion has ten UN 1/2" threads (including 1/2-28), SW has 1/2-13 and 1/2-20. Either of them are configurable though so it's not like it's a problem. Which thread are you missing? The only thread I've come across so far that Fusion didn't have is for a C-Cell tube (1 3/32-20) which to be completely fair isn't even listed in the Machinery's Handbook. Actually I'm pretty sure Fusion's library includes every thread listed in the Machinery's Handbook up to 4". |
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Originally Posted By Blob: Fusion's included thread library is huge. Way larger than the standard thread library that came with my copy of solidworks. Fusion has ten UN 1/2" threads (including 1/2-28), SW has 1/2-13 and 1/2-20. Either of them are configurable though so it's not like it's a problem. Which thread are you missing? The only thread I've come across so far that Fusion didn't have is for a C-Cell tube (1 3/32-20) which to be completely fair isn't even listed in the Machinery's Handbook. Actually I'm pretty sure Fusion's library includes every thread listed in the Machinery's Handbook up to 4". I'd have to look and see what I'm currently missing. Last time I was messing with threads on f360 it was missing stuff like 1/4-28 UNF or 1/4-80, 1/4-120. Things that are extremely common in my world, they are readily available ultra fine threads and nothing special. My lathe will do those and it's from the late 1940s. I don't think it had 1.375x24 (large HUB thread). Than again, SW also didn't have 1.375x24. I'm also not sure why f360 defaults to 100° for English counter sink when clearance holes are done. 82° is standard. Just more things I have to look for and go through menus screwing up the flow. At least SW remembers the last thread I used and sets that in the hole wizard. |
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Originally Posted By Deerhurst: I'd have to look and see what I'm currently missing. Last time I was messing with threads on f360 it was missing stuff like 1/4-28 UNF or 1/4-80, 1/4-120. Things that are extremely common in my world, they are readily available ultra fine threads and nothing special. My lathe will do those and it's from the late 1940s. I don't think it had 1.375x24 (large HUB thread). Than again, SW also didn't have 1.375x24. I'm also not sure why f360 defaults to 100° for English counter sink when clearance holes are done. 82° is standard. Just more things I have to look for and go through menus screwing up the flow. At least SW remembers the last thread I used and sets that in the hole wizard. Fusion has 1/4-28. Does not have -80 or -120 by default, but again can be configured in the .xml thread table easily. I added 1/4-80 to the table using data from machining doctor. It took me longer to look up the thread data and write this post than it did to add the thread to the table. Attached File Attached File Attached File Changing the 100 degree to 82 is just clicking an option in the drop down, no different than changing an option from counterbore to countersink. It also remembers the last size used. I know you love to hate on fusion at every opportunity but it sounds like you're grasping at straws here. |
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Originally Posted By Blob: Fusion has 1/4-28. Does not have -80 or -120 by default, but again can be configured in the .xml thread table easily. I added 1/4-80 to the table using data from machining doctor. It took me longer to look up the thread data and write this post than it did to add the thread to the table. https://www.ar15.com/media/mediaFiles/160722/Screenshot_2026-03-15_105523_jpg-3729991.JPG https://www.ar15.com/media/mediaFiles/160722/Screenshot_2026-03-15_105500_jpg-3729992.JPG https://www.ar15.com/media/mediaFiles/160722/Screenshot_2026-03-15_110739_jpg-3729997.JPG Changing the 100 degree to 82 is just clicking an option in the drop down, no different than changing an option from counterbore to countersink. It also remembers the last size used. I know you love to hate on fusion at every opportunity but it sounds like you're grasping at straws here. Across multiple machines F360 has NOT remembered the last thread I used. Always reverts to metric every single time I go to add threads. Im forced to use F360 professionally. Its been a BIG slow down in our development/CAD work vs solidworks. To make matters worse it is primarily on mac which makes things more of a struggle in an engineering department plus the non standard way autodesk installs f360 on mac. The mac thing and the price were likely the only considerations by upper management and even the price has gone up at least 30% in the short time we've had it. The fact f360 defaults to non standard options, such as 100deg is another step required. Not a big deal for the hobbiest but when you spend 8hrs a day dealing with it and constantly having to change little things that should stay constant it becomes a real pain in the ass. Every time I add a tapped hole I have to select that its a thread, then go back to ANSI Inch then find the thread I want. At least they have the thread number (#10) in there instead of making me remember the tap drill diameter to choose my thread, now. Always defaults to the same metric whatever every time I use the hole tool. I dont think Ive ever done a metric hole in f360. At one time the custom threads were not kept across updates. We did have some fine thread customs in there at one time but lost all of them over some update. Has this been fixed? |
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well I kinda sorta did it.. now to get the measurements for the exact location of the thread, size of it and pitch.. ugh. lol  |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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well after quite a few "practice runs" I have creating the thread down fairly well. My problem is I can't figure out how to move the coil closer together. I need to move the bottom one up. 
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To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By -Obsessed-: Did you follow my guide that I gave you? What you're looking to adjust is the thread pitch. ETA..if I change the pitch it moves the top part of the thread down.. |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By Striker: I'm slowly loosing my mind. Why is it doing this?  https://www.ar15.com/media/mediaFiles/135/complete_lid_6_v1-3738294.jpg I think I know what is causing it and if that is the problem I can't seem to correct it. I'm thinking it's the position, angle of my thread profile that is messing up. Although the last attempt had the thread inside the lid but it was in further on one section and the opposite section the threads weren't bonded to the lid. When I insert the single coil I make sure to line the center circle with the one in the origin. It's like fusion isn't drawing a perfect circle. |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By Striker: still struggling with this. I think I know what is causing it and if that is the problem I can't seem to correct it. I'm thinking it's the position, angle of my thread profile that is messing up. Although the last attempt had the thread inside the lid but it was in further on one section and the opposite section the threads weren't bonded to the lid. When I insert the single coil I make sure to line the center circle with the one in the origin. It's like fusion isn't drawing a perfect circle. Is the lid centered at the origin? Share the link to the file and I can take a look at it tonight |
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Originally Posted By Blob: Is the lid centered at the origin? Share the link to the file and I can take a look at it tonight I'll double check but I'm pretty sure it is. |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By -Obsessed-: Are you using the vertex of the triangular cross sectioned coil as the guide curve and the face of the coil as the guide surface? I think I may have it sorted out. Doing a test print now. Hours of trying to print a replacement lid for a used juice pitcher my future daughter in law bought. lol |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Originally Posted By Striker: I did initially but for some reason I can't click on the vertex now. Just the face of the outside of the coil. I think I may have it sorted out. Doing a test print now. Hours of trying to print a replacement lid for a used juice pitcher my future daughter in law bought. lol Thats your issue. You need both to keep the profile running true and at the proper pitch. Just an annoying aspect of Fusion. All CAD have these annoyances, theybare just different. You'd kick yourself if you saw how easy this is to do in SolidWorks.
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Originally Posted By -Obsessed-: Thats your issue. You need both to keep the profile running true and at the proper pitch. Just an annoying aspect of Fusion. All CAD have these annoyances, theybare just different. You'd kick yourself if you saw how easy this is to do in SolidWorks. The first time I followed your tutorial it worked fine. Now it doesn't. lol |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
well the thread is inside the lid but didn't bond in one section.. it's thinner where it's bonded which tells me it isn't centered correctly.. 
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To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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I found a glitch..maybe.. I'm still fighting with positioning the thread in the correct spot and I was messing around with the section settings and discovered this.   Then this happened. I didn't move anything. 
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To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.
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Well I solved my problem and decided that food safe pla is a PITA. I made the part of the lid with regular PLA and printed the top of the lid with the food grade. The dark blue is the food grade. No matter what I tried the food grade would "stick" to the glass jar. I printed the exact file using regular pla and it worked great.  |
To say that you are on thin ice would be a vastly optimistic view of your current situation. The ice has melted. You are being supported by the surface tension of water.