Tips/Tools for machining large diameter threads on mill

[Elemental_Garage]

if your hole is modeled to major diameter, how are you roughing and finishing it to the correct minor diameter size?
i wouldnt fuck with the PDO for wear offset, if you need slightly larger, do that in the stock to leave area.

I wasn't. I did the hole thread milling on a 2.375 hole, which is likely why they're so darn tight. So both boss and hole were at major diameter.

 

[Elemental_Garage]

Internal thread- mill hole to minor diameter, thread mill to major diameter
External thread- mill boss to major diameter, thread mill to minor diameter

So I feel like the problem is coming in because you have a cylinder or cylindrical hole in CAD, and it can't simultaneously be at the major and minor diameter. So either the milling or the threadmilling path will need to be offset. Or both, but one will be offset far more than the other.

I thought you said both are modeled to the nominal 2.375" diameter. But if that's not the setup, then what I write below won't be quite right.

Internal thread, you need to cut the minor diameter significantly smaller than that (closer to 2.3-2.31), and use a small PDO on the threads to get it to gage right, .020 minimum by my calculation for a pointy tool. And that's effectively zero clearance. I think you will want .030 to .040. So to check clearance, 2.375+.04-2.31=.105. This is less than .388-.25=.138, so it won't rub.

External thread, you would mill to a bit below nominal (maybe about .01 below) and use a rather large PDO to get the threads to depth. I would probably model the boss at 2.365 and drive both milling and thread milling off of that. You want the threads to cut to about .126 below your major diameter and would use this for PDO. As you can see, .126 is getting near .138. Here, a PDO of .138 is when things will rub.

The Harvey tool comes to a point. I think this is why there is slight disagreement between my numbers and Saunder's numbers, plus I think you want more clearance than a "2B" thread. I agree that the "tooth height" would seemingly make more sense to be 1/2 of .138, but I want to emphasize this isn't evidence of a math error or clearance problem, just some disagreement over terminology. PDO is a diameter offset and trouble arises when you run out of diameter offset between tooth and shank. If PDO is .100, the tool cuts .05 more radially.

Thanks for this explanation and modeling. I'll reread it again in the AM when I'm more awake to ensure I understand it, and may do some test cuts tomorrow to give this a go.

One other question that's top of mine. When threading a through hole do you normally tell it to thread past the bottom of the hole? And ideally chamfer after the thread cuts?

 

[empower]

I wasn't. I did the hole thread milling on a 2.375 hole, which is likely why they're so darn tight. So both boss and hole were at major diameter.

you made the hole 2.375" ID for a 2.375 internal thread? i'm so confused.

 

[???]

A quick and dirty thread mill is to grab a lathe thread boring bar in a milling tool holder. Use a full form insert and mill your male thread first. If you start with extra stock it's easy to measure the OD and to tweak it with the full form inserts. Added bonus is the same tool can be used in the lathe.

 

[dodgin]

Thanks for this explanation and modeling. I'll reread it again in the AM when I'm more awake to ensure I understand it, and may do some test cuts tomorrow to give this a go.

One other question that's top of mine. When threading a through hole do you normally tell it to thread past the bottom of the hole? And ideally chamfer after the thread cuts?

I chamfer everything beforehand.

For Ingersoll tools we use a local distributor. It should be pretty simple for someone who is at least moderately resourceful like yourself to track down an Ingersoll rep who will probably be more than willing to let you demo some tooling.

 

[Elemental_Garage]

you made the hole 2.375" ID for a 2.375 internal thread? i'm so confused.

Yes. Mistakes were made.

 

[empower]

Yes. Mistakes were made.

takes a man to admit his mistakes, kudos.

if you're the one modeling the parts, i always model internal threaded holes to the minor diameter, use 2d contour to finish that to correct minor size. then use PDO in the threadmill path so that it cuts it to the right major diameter. opposite for external threads - model to major size, use PDO in threadmill path.

also, use wear comp and walk up to the right size using the wear offsets in control.

 

[Elemental_Garage]

takes a man to admit his mistakes, kudos.

if you're the one modeling the parts, i always model internal threaded holes to the minor diameter, use 2d contour to finish that to correct minor size. then use PDO in the threadmill path so that it cuts it to the right major diameter. opposite for external threads - model to major size, use PDO in threadmill path.

also, use wear comp and walk up to the right size using the wear offsets in control.

Never going to learn if all I get are wins. Losses make the lessons.

So use PDO to push to the major diameter, but then if the fit is too tight still use cutter comp to slowly cut deeper to provide relief?

 

[empower]

Never going to learn if all I get are wins. Losses make the lessons.

So use PDO to push to the major diameter, but then if the fit is too tight still use cutter comp to slowly cut deeper to provide relief?

bingo!

 

[mr_servo]

I started to get into this last night, but didn't want to confuse the issue even more. It is safer to model the internal thread at the minor diameter. Why? Because some chucklehead machining without taking a careful look at the drawing won't scrap the part. Drill a M3 hole where there's supposed to be an M3 thread, and the part is toast. If I'm sending a drawing out for quote, it always has internal threads modeled at the minor diameter. For internal stuff, sometimes I get lazy. Often I will just tell HSMWorks the major diameter I want for an internal hole (using the drill feature), but this leaves out the G41/G42 offset codes so I either have to add them back in manually or change the offset and repost. One reason I keep some notes about what's worked in the past.

This approach sorta loses the educational aspect of often needing to threadmill an internal thread beyond the major diameter due to the sharpness of the cutting tool. I have a big spreadsheet for calculating this stuff. It's not easy to use, the tolerances bands are for metric threads, and it's not really something I want to share with the world. But the numbers I was spouting off come from a close look at thread forms and acceptable tolerances.

If you do this thing of modeling the external at the major and internal at the minor diameters, it allows you to just cut the pocket or boss to size and it will likely be close enough. You will then need a large enough PDO to make the pitch diameter correct. And it should be noted that you do not want the PDO to be equal for the two cases (internal vs external). The proper distance from root to crest is not the same for both.

So, post here which approach you would prefer to take and I'll try to get you some numbers with a reasonable likelihood of working on the first shot.

 

[Elemental_Garage]

I think conceptually it's easiest for me to remember to start with major for an external, and minor for an internal, and work from there, at least until I get more experience. I've only been at CNC in general for a few months and threading (aside from rigid tapping) for about a day and a half .

 

[empower]

I think conceptually it's easiest for me to remember to start with major for an external, and minor for an internal, and work from there, at least until I get more experience. I've only been at CNC in general for a few months and threading (aside from rigid tapping) for about a day and a half .

you've got the right attitude, keep at it, you'll get much better with no time.

 

[mr_servo]

I think this picture will help a lot to see how all this comes together. I put the external thread major diameter at 2.365 and the internal thread minor diameter at 2.300. Regardless of the clearance, the internal thread PDO comes out to .108 and the external thread PDO comes out to .126 if you're cutting with a sharp tipped tool. You can see this comes about because the flat widths are different for inside and outside.

Given the application, I think you want even more clearance for the reasons stated before. But you can leave PDO alone and increase clearance just by moving the major diameter of the external thread or the minor diameter of the internal thread, and the threading operation will follow.

Thread standards often allow a sharp tip on the internal thread and don't allow it on the external thread. This is why a single form thread mill will be advertised for internal use but not for external use. On a highly stressed bolt, this matters. On a coolant cap, not so much.

And with that, I wish you luck on good threads on the 2nd try!

 

[Elemental_Garage]

Thank you for all the help, numbers, and diagrams all!

@mr_servo you mentioned plastics earlier and I'm definitely considering this too, especially for the light-weight builds in the future. I started with 3D printing before moving into CNC and do have access to print some high-temp (relatively speaking), chem resistant materials. I can't do PEEK yet, but would love to in the future. Those printers tend to be nearly used CNC money though. In fact, I'll be printing the o-rings for this container, and the light-weight version will likely be all plastic too.

I'm really enjoying the vertical integration of being able to make stuff in multiple materials and combine them when needed.

 

[kenton]

You can machine your cap out of plastic.

 

[Elemental_Garage]

You can machine your cap out of plastic.

True too. I just like how there is comparatively little setup to 3d print it. I can put down a little glue, close the door, hit print, and kick out 10 if I need. I know I could get there machining it, but then I need to setup the vises, soft jaws, etc. for that. But always good that I have a backup if needed.

 

[kenton]

Use the same setup, program and, tooling as your aluminum cap, make a few of each if you want.

 

[magno_grail]

You could use a 60 degree double angle chamfer cutter instead of a thread mill cutter. A lot more clearance between the shank and cutting tip.