Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

A (math heavy) investigation of a thread mill toolpath - relationship between stepover # and radial tooth engagement

8 REPLIES 8
SOLVED
Reply
Message 1 of 9
t.g.mandel
243 Views, 8 Replies

A (math heavy) investigation of a thread mill toolpath - relationship between stepover # and radial tooth engagement

In an earlier post (https://forums.autodesk.com/t5/fusion-360-manufacture/controlling-varying-the-stepover-of-multiple-r... ) I was looking for a way to control the radial depths of cut, or at least the initial one relative to my chosen stepover.

 

One answer given (thank you @seth.madore), as to how F360 works, was as follows:

 

"Your stepovers are calculated back from your (background calculated) Pitch diameter offset. It will only give you as many passes are possible before the toolpath collapses in on itself. There will be a warning if you've defined more passes than are possible, but the toolpath will still run with as many passes as it can fit"

 

I wanted to investigate this further, in hopes of better controlling the amount of tooth engagement with the first pass into the hole wall when using a single form thread mill. I have summarized my investigation in a table in hopes that 1) others might verify that the my methodology and calculations are correct, 2) it confirms my belief that there may be a way to use these calculations to program an appropriate/effective initial radial depth of cut, and 3) it might interest others to see how changing the number of stepovers impacted the initial radial depth of cut.

Note: I made a model of the thread mill tooth in F360 and used it to measure the areas to get the % of tooth engaged

 

I appreciate any insights people have the time or interest to offer.

8 REPLIES 8
Message 2 of 9
hackish
in reply to: t.g.mandel

Your work looks good to me. I did some work on this topic but never finished. It looks like you were doing it experimentally on the machine whereas I approached it by parsing the G-Code to calculate the radial distance from the hole centre (which I set to G54 for ease). I theorized that optimizing the tooth engagement for less deflection would result in a nicer thread, but I wasn't able to demonstrate that because I didn't have an adequate means of precisely measuring the resulting thread. My feeling is that the last cut was made as a finishing pass and any leftover material was cleaned by this. It might be an issue in deep holes with a longer cutter. I wasn't able to figure out a way to dynamically control the stepover, so I set the idea aside for now.

Message 3 of 9
t.g.mandel
in reply to: hackish

Thank you for taking the time to look at my data and share your thoughts and your own methodology. I got the data - slowly - by setting the simulations as slow as possible, and watch/recording the max/min x values as the cut progressed - happily the data confirmed my readings were correct in that the stepovers matched those programmed. I feel I can use my results to help me decide on a combination of stepover # and radial cut depth that has an initial cut that won't break my thread mill, but at the same time that has subsequent stepover cuts that are cutting chips and not rubbing metal. Thank you again.

Message 4 of 9
leo.castellon
in reply to: t.g.mandel

I don't know if you are aware of this, but many thread mill manufacturers provide thread mill calculators. We use a lot of Scientific Cutting tool thread mills and here is some relevant information that they provide with a link to the thread mill generator: tm_sptmun.pdf (sct-usa.com) and Thread Mill Code Generator – Scientific Cutting Tools, Inc. (sct-usa.com) . 

 

LeoC

 

Message 5 of 9
t.g.mandel
in reply to: leo.castellon

Thank you for the resource. I actually am using a SCT single form thread mill as my first one - I had not seen that resource on their site.

It certainly does what F360 (currently) can't do, and that is allow me to choose different radial depths of cut, with a different % for each. For me the benefit of staying with F360 is that I can learn to program all the other useful parameters, and have an easier way to save and compare any changes I make. I am new to CAM, and still learning F360, but it may benefit me to stick to one method. Having said that, I did use the linked code generator to create a gcode file, and I may set up my machinable wax block to run a few tests and see how it works with my controller. My inexperience has me wondering if it is as simple as loading the generated gcode file into my controller and hitting cycle start (making sure things like tool #s and WCSs are correct. Thank you again for offering an alternative for me to try.

Message 6 of 9
leo.castellon
in reply to: t.g.mandel

I can understand trying to keep everything within Fusion, but don't go down the rabbit hole in overanalyzing this. Yes, ideally, the thread mill should go into the material at different percentages, but realistically, the way the tools work, just go with number of passes, be conservative, it might not be perfect, but it will still work and won't wreck your tool. This same exact issue will happen when you go into lathe thread programming, Fusion will just ask for number of passes, not percentages. 

 

If you still want to machine your threads by percentages, there is an easy solution. Program the thread mill operation with a stock to leave based on the percentage that you want, one pass. Copy and paste this operation and change the percentage and then repeat as many times as required. It is a little more time consuming for you to program, but easily done.  For example, your first operation will leave .040" stock to leave, second operation will leave .020" and so on.

 

One thing I strongly recommend is that after completing a thread milling operation with your specific tool, and making sure it works, save that operation by storing it as a template.  Personally, with my luck, I have never been able to program a thread milling operation and get it perfect the first try, I always have to add cutter comp to get the thread gauge to fit properly. I then go back into Fusion and modify the program taking into account how much cutter comp I had to add. 

 

LeoC

Message 7 of 9
t.g.mandel
in reply to: leo.castellon

Great advice, especially for someone like me with little machining experience - and a tendency to dive into rabbit holes😀 . I will make note of your creative solution for % passes, and will definitely start saving toolpaths that work as templates. Thank you again for your support - I appreciate it.

Message 8 of 9
leo.castellon
in reply to: t.g.mandel

You will save a huge amount of programming time by using templates. Program a part, run it on your machine, see how it works, if you have to override feeds and speeds on the controller, make note of the changes. Go back into Fusion and modify the speed and feed changes that you made on the controller and change those settings in Fusion. Save the operation as a template, Then, next time you need to program for something using the same tool and material, you have it all figured out and all you will have to do is change the geometry. No need to start from scratch and guess what speeds and feeds will work. This applies to all of the machining options in Fusion, drilling, surfacing, lathe operations, everything. You took the time to do your research, determined what tool you were going to use, how to hold the part, what depths of cut to use, how much to take off radially and how your machine reacted to those settings. You might have a desktop machine or a behemoth of a machine, you figured out the original parameters that work, save them, don't waste time by not saving them. Then on your next part, go to the setup tab, right click on it, and choose "create from template", import it into your operation, select your geometry, and voila, you are done. 

 

LeoC

Message 9 of 9

I came across this today linked from another machining forum: EMUGE-FRANKEN USA on Instagram: “Drill / thread mill / chamfer all-in-one tool! Tool: Emuge-FRANKEN ...

 

LeoC

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums