1/4 NPT thread mill

[mikechvz]

I have a 7 tooth insert and a taper tool holder for the 1/4 NPT, my customer wants me to go -.570 depth finish. When i program the thread mill tool path and set anything more than 1 cutting tooth, it does it in multiple depth cuts. Wont this interfere with the taper finish for this thread?

[Guyinthedesert]

No, as long as you've got the taper angle set in the threamill parameters, it'll come out right

[FROZEN]

Taper angle in tool parameters on X4???X7 has it.

[mikechvz]

so even though the tool holder itself has some taper, i still need to fill in the "taper" box in X4?

[Guyinthedesert]

so even though the tool holder itself has some taper, i still need to fill in the "taper" box in X4?

 

Yes, because the actual toolpath is a spiral, not a helix

[mikechvz]

i figured 1degree47 minutes is equal to 1.79 degrees so im gonna try this out, i appreciate the input

[crazy^millman]

Yes since the taper on the tool is only part of the code, the taper box lets the operation know you are cutting taper threads with that tool.

[Matthew Hajicek - Singularity]

I do these pretty much every day in H13. Here's what I do:

 

[mikechvz]

thanks

Matthew Hajicek™ -Midland Tech

[Rick46]

We use carmex solid carbide threadmills with the taper on the cutter and don't have this worry with inputting the taper in the taper angle box..just curious what brand tooling are you using that has 13 teeth or are u counting every tooth on the cutter if so that sounds like a low amount..I find using 1 tooth to work better and to enter cut by start at top of hole and to enter and exit at center rather then leading in and out of hole with radius to prevent accidental gauges..I know it's climb cutting this way but less hastle and retracts in my opinion also some controls will error out with a arc lead in with wear turned on..I've been cutting threads for long time and all different sizes and pitches and find this method to be sure fire every time and great finish..doing it the way above I can see why people are intimidated by thread cutting and why everyone that runs across a job that requires thread cutting comes to me for advice..all about the right tooling and cutter dia.'s as well as the way you approach it and it's as easy as drilling the hole to be thread cut

[crazy^millman]

I know it's climb cutting this way but less hastle and retracts in my opinion

 

Sorry, but do you mean conventional cutting? I have cut my share of threads as well and I have to disagree 100% with your statement. I have cut threads in well over 20 different materials in many different sizes I cannot even count and I always start the bottom on right hand threads when thread milling Even when we use to have to draw the Helix and Center point them Back in V7 not X7. Before that I use to use Macro programming and I still cut from the bottom even on NPT thread back in the early 90's. You would be surprised how much better the surface finish would be and the ability to hold size on hard material will be cutting it climb verse conventional. Sorry just been my and many others I know experience.

[Rick46]

Yes I meant conventional cutting sorry got my self mixed up in long post. Yes I agree climb cutting is best way to go but I don't like the plunge to the bottom of the hole and working it's way up. Just a personal preference I guess when thread milling..

[peon]

I also use the Carmex NPT threadmills that include the taper on the flutes and have NEVER added the taper angle in the toolpath parameters. Is this value only required when multiple depth cuts are needed?

[Guyinthedesert]

I also use the Carmex NPT threadmills that include the taper on the flutes and have NEVER added the taper angle in the toolpath parameters. Is this value only required when multiple depth cuts are needed?

 

Yes. Look at it this way. Say you have a tapered threadmill, and the bottom tooth has a diameter of .200 (I'm just using BS values here for the point of illustration) Say the next tooth up from the bottom has a diameter of .250. If your toolpath just makes a helix up one turn, your bottom tooth is going to be .025 away from where the "next to bottom tooth" left off. So the toolpath needs to spiral outward as it goes up. This is controlled by the taper angle.

 

I'm curious what your threads looked like without the taper angle In the toolpath. The threads would still have a taper, from the taper in the tool, but it seems there would be a discontinuity in the thread.

[crazy^millman]

Peon, I am sorry to say, but you have been cutting thread wrong for a long period of time. Like Guyinthe desert said, that taper has to be accounted for when cutting the thread, yes he tool has it, but I would think you are not cutting correct threads. On smaller threads you may not be seeing since the error is so small, but try it out on a 3" NPT ot 6" NPT and tell me what you see?

[jeff]

Peon, I am sorry to say, but you have been cutting thread wrong for a long period of time. Like Guyinthe desert said, that taper has to be accounted for when cutting the thread, yes he tool has it, but I would think you are not cutting correct threads. On smaller threads you may not be seeing since the error is so small, but try it out on a 3" NPT ot 6" NPT and tell me what you see?

 

I've never entered an angle either. Although I'm only doing 1/8" and 1/4" NPT's. never had one rejected and the gage fits fine.

Just tested this out Friday, I couldn't tell a difference in gage feel or size, but like I said, it was only an 1/8" NPT I was cutting.

Definitely going to start using the angle though, just in case

[peon]

Damn, I've been threadmilling NPT for water lines in our molds for years with excellent results and never had an issue. I'll have to add the taper values to my templates and make the machinist aware of the issue. The most common sizes I mill are 1/4-18 and 3/8-18 and rarely go larger. Now and then we will threadmill 1/2-14. THANKS FOR THE HEADS UP!!!

[GoetzInd]

If you are not putting in the taper it will not taper out as it does the pitch helix. Gaging may still go if you open it up a little further but the thread form is not correct. I bet it would leak on a dry seal form but have never tested it out.

 

Mike

[crazy^millman]

Well think about it. There is an anlge on that thread and if you are cutting straight up you are in reality you are cutting a straight thread that just happedns to have taper on the outside of the tool. You do not see the error as much becuase of the taper on the tool ,but what ever you would do with a single point tool to cut a thread is the same way you would cut with a multi-flute tool. 23 years ago we dod not have all the options we have today. To cut threads with a tool like this where I cam from was crazy to even think about, much less do. I puy my job on the line at one company. They had hard face welded some housings. The threads in the housings got messed up and could not be fixed with a tap. The Power Company they were for sent out all types of engineers and they were going to scrap 30 housings at $300k each. I walked over in my early 20's and told them to threadmill them and they will be fine. Everyone includeing the owners and shop foreman called me crazy. I told them I knew it would work I had been doing it for years. Owner was a 30 year conventional machinist and said it could not be done. I told him if it would not work I would quit. The engineers laughed at me and told the owenrs unless that had $3.6 Million to replace them they might need ot listen to me. I went and borrow the tool from a company I use to work with and we cut all 30 with one tool. I got to keep my job and they got the parts out and the city was not going without be hurting for power for 6 weeks since that was how long it was going to replace the housings.

 

Get away from the mutli-flute tool and go back to basics and think about a single point tool. That along should should show anyone cutting taper threads without taper is just asking for trouble.

[Scott Lundin Shopware Inc.]

Even if your tool has enough teeth vertically to cut the tapered thread in one circular move around the hole you should still set the taper angle. For a 1/2-14 NPT with 1.783 degree taper, the tool would rise .0714 in. in the Z-axis during one circular move around the hole. This would be a difference of .0022 in the X-axis assuming you started and ended at 3:00. Look at your output g-code, the X and Y moves should be expanding outward as the tool feeds upwards.

[crazy^millman]

Scott, yes that was a perfect picture and why you would need to be cutting using the taper.

 

We use to make tapered repair studs for the paper mills and for power generation. The BoilerMaker would take different tapered tapes and retap a standard hole till the parent Material was fully seen again. They would then mark the tap on the deepest hole they had to tap and then tap all holes on the housing to that depth.

They would then send us the the depth and taper angle of that tap. We would then tap a brass ring with that tap to the same depth on the tap. We would then make threaded stud with the same Standard threads they had, but with that taper angle threads on the other side. Everyone one had to be check and could not vary more than .005 on height when screwed into place. .005 seems like a lot of tolerance, but when dealing with Tapers that is nothing .0003 was our tolerance cutting these threads and we would normally scrap about 5% on a run making these things.

 

Taper is important and yes Mike I think on a Dry Seal Thread over time it would fail.

[Rick46]

If u start at top and cut to bottom with a cutter that has taper using it as one cutting tooth it won't need the taper angle only if you get fancy with multiple teeth and step down engagements.

 

The seal is better than with threads cut with a hand tap. They will dry deal fine but we use thread tape just as a common practice on all pipe plugs..

[Rick46]

NM lol

[Rick46]

I think the best answer would be to listen to your tool supply company on how to properly run the thread mill weather the taper degree need me included or not and a lot of this also depends on what software you use to generate your code for the thread mill path. but I do no the carmex npt thread mills are full form thread mills that include the taper on them and can be run like cutting a screw thread to achieve your npt thread needs. I also know now after some research there are thread mills out there that do not have this feature and do need the taper degree box filled out with the 1.78 degree on it when using the thread mills that are not designed to be run straight down to form the threads. and again software also plays into this so In my opinion I would talk to the tool sales rep and see what their recommendations are.. as all have said technology has changed and they do make multi tooth as well as inserted cutter thread mills for npt threads that cut the angle for you using a straight down tool path motion without needing the tool taper degree included in your software if your software has this option available. just because an option is there doesn't mean it has to be used. its there to compensate for tooling that doesn't include the angle when forming the threads..

[BestMastercam]

Well think about it. There is an anlge on that thread and if you are cutting straight up you are in reality you are cutting a straight thread that just happedns to have taper on the outside of the tool. You do not see the error as much becuase of the taper on the tool ,but what ever you would do with a single point tool to cut a thread is the same way you would cut with a multi-flute tool. 23 years ago we dod not have all the options we have today. To cut threads with a tool like this where I cam from was crazy to even think about, much less do. I puy my job on the line at one company. They had hard face welded some housings. The threads in the housings got messed up and could not be fixed with a tap. The Power Company they were for sent out all types of engineers and they were going to scrap 30 housings at $300k each. I walked over in my early 20's and told them to threadmill them and they will be fine. Everyone includeing the owners and shop foreman called me crazy. I told them I knew it would work I had been doing it for years. Owner was a 30 year conventional machinist and said it could not be done. I told him if it would not work I would quit. The engineers laughed at me and told the owenrs unless that had $3.6 Million to replace them they might need ot listen to me. I went and borrow the tool from a company I use to work with and we cut all 30 with one tool. I got to keep my job and they got the parts out and the city was not going without be hurting for power for 6 weeks since that was how long it was going to replace the housings.

 

Get away from the mutli-flute tool and go back to basics and think about a single point tool. That along should should show anyone cutting taper threads without taper is just asking for trouble.

 

100% agree with you.