Thread milling

[ErnieD]

I am thinking about doing some thread milling and would like to know if I can use multi thoothed thread milling cutters with PP other than the the single tooth ones . Any thoughts ?

Similar Threads:

• Need Help!- Thread Milling
• Need Help!- Thread milling a 1/8-27 npt internal thread
• Need Help!- New to thread milling
• Thread Milling
• Thread milling

[TurboStep]

I am thinking about doing some thread milling and would like to know if I can use multi thoothed thread milling cutters with PP other than the the single tooth ones . Any thoughts ?

You certainly can.
Step

[jwatte]

As long as the pitch on your threads matches the cutter, that will work fine. I use a Sandvik M2.5-0.45 thread mill with three teeth and it's great!

[Tigster]

I purchased a cutter for this purpose and, being also someone who finds the conversational programming a bit confusing (I got my feet wet in CAM before PP/conversational) and it's just a bit confusing. I know it's meant to be simple, maybe I ate a lot of paint chips as a kid, at any rate, it's not real clear for me either. Anyway Ernie, I'm right with you on both!

[vmax549]

Tig if you want I can explain the process for you. Once you understand the process it is easy to use.

(;-)

[TurboStep]

I'd suggest watching all the PathPilot videos you can find on Youtube. There are plenty of good ones out there and you can probably learn something from each.
General PP (including a quick thread mill run though):

Thread mill specific:



From Cliff, Part 1



Part 2




Step

[Tigster]

Thank you VMAX and Turbo, I did run through a conversational setup for it, went smoothly (this was PPhub)...in reality will I explode my cutter? Who knows? TBH the main concern I have is the setup (tool offset and F360 tool setup -when I use CAM instead) It's an odd tool to setup...for me anyway.
Oh Man Turbo, I just noticed your in Switzerland. I'm uber jealous! My wife and myself took a train through Germany and Swizerland for a month. FEEL. IN. LOVE. with your country...#1 on our list!

[mountaindew]

. I know it's meant to be simple, maybe I ate a lot of paint chips as a kid, at any rate, it's not real clear for me either.

When in doubt air mill it!

Not much in the cnc or machine tool world is simple. Over time you develop an understanding of how things work, what math applies and what strategy might work best.
imho most cam software will make you want to eat paint chips! Maybe others master this overnight and some cam or conversational is better then others! I l-earn every step.

I spent a number of hours recently just sorting out what values do what in cam lathe tool tables. I was about to go scjcdn-08a nuts! Anyway it took time and persistence just to learn how to correctly and accurately enter or edit the values for one little part of the cam bloatware "tool table" for lathe operations. So I dont think you lack any special skill! In fact I find cad, cam and cnc tool operation to be a perishable skill. You need to build and refine your process to have confidence. Otherwise Mr bozo is going to be visiting.

I even turned "air" recently! Not because of cam output, But I was not confident in the lathe tool table offsets "I setup" in PP
Something I have not done on mill in a long time and ever on router .

[ErnieD]

Maybe I was not clear as to what I wanted to know . I was thinking of the thread mills that are similar to a tap . Move to the bottom of the, hole feed to thread depth , make one revolution , feed to center then out .

[TurboStep]

Thank you VMAX and Turbo, I did run through a conversational setup for it, went smoothly (this was PPhub)...in reality will I explode my cutter? Who knows? TBH the main concern I have is the setup (tool offset and F360 tool setup -when I use CAM instead) It's an odd tool to setup...for me anyway.
Oh Man Turbo, I just noticed your in Switzerland. I'm uber jealous! My wife and myself took a train through Germany and Swizerland for a month. FEEL. IN. LOVE. with your country...#1 on our list!

A month! Well I guess you must have liked it The grass is always greener... but I can think of worse places to live...

I doubt you'll explode your cutter. Run the cut a couple of inches above the hole first to make sure you're comfortable before cutting the thread and I'm sure you'll be ok. Before I bought my Tormach I tapped a whole load of 2mm threads by hand and got really sick of trying to dig out broken taps. I therefore started thread milling on my second ever part and never looked back. I've only broken one thread mill and that was just due to a dumb move on my behalf, nothing to do with the thread milling process itself.
The only aspect you should look out for is the feed rate. While the cutting takes place around the outside diameter of the thread, the center of the cutter only rotates on a very small circular path inside the hole (think of a .18" peg rattling inside a .25" hole, the center of the peg will rotate around a circle .25"-.18" = .07"). The cutting feed rate, as seen at the outside diameter will therefore be much higher than the feed rate programmed for the tool path. PathPilot Conversational automatically drops the actual programmed feed rate to compensate for this. If you pause the PP simulation while the thread is being cut you will see that the actual feed rate is much lower than the feed initially set in the conversational field. It can obviously also be seen in the G-Code. Fusion doesn't compensate automatically so you will have to adjust the Cutting Feedrate accordingly.
Step

[mountaindew]

Maybe I was not clear as to what I wanted to know . I was thinking of the thread mills that are similar to a tap . Move to the bottom of the, hole feed to thread depth , make one revolution , feed to center then out .

In my cam cam you set everything here.
Dont know how to set PP conversation to do this but someone does!

[vmax549]

Yes PP can do that it is all in teh settings. You program teh tapp to go as low in hole as you need (depends on teh length of the threadmill)as start point then you program the depth as startpoint + threadpitch . That will make PP program 1 helical move the depth of the threadpitch. Startpoint ------>> to endpoint . I tried it to make sure (;-) IF the threads on teh threadmill are not long enough then you add more depth (rotations of teh helix) to get a deeper thread. IF there is clearnace on teh top of the treadmill points.

(;-) TP

[metalmayhem]

it might be easier and quicker to throw in some simple hand code
for example

G0G90G54 X0Y0S5000
G43H1Z1.
Z.1
G1Z-1.F15.
G91
X-0.05
G3I.05Z.1
G1X.05
g90
G0Z.1

if you have multiple holes then you can create a sub routine , copy paste the previous drill cycle for your positions and add a sub call for each position

[mactec54]

Maybe I was not clear as to what I wanted to know . I was thinking of the thread mills that are similar to a tap . Move to the bottom of the, hole feed to thread depth , make one revolution , feed to center then out .

I had the same thoughts as I'm not sure they understood the difference between a real thread mill, and single point thread mills which can have a different number of cutting edges but is still a single point cutter it appears there conversational programming is only for single point threading

You could program it for that type of thread mill and see if it can do it, dry run the program in the control you will soon know if it can do it or not

[mactec54]

it might be easier and quicker to throw in some simple hand code
for example

G0G90G54 X0Y0S5000
G43H1Z1.
Z.1
G1Z-1.F15.
G91
X-0.05
G3I.05Z.1
G1X.05
g90
G0Z.1

if you have multiple holes then you can create a sub routine , copy paste the previous drill cycle for your positions and add a sub call for each position

This is how you would use and program a ( 1 ) pass thread mill



T1M 6 ( Tool change )

S1200M03 ( Spindle on )

G0G90 X 0.0000 Y 0.0000 M08 ( Start point )

G43 H01 Z0.1000 ( Rapid above part )

G1Z- 0.50F50. ( Feed to depth )

G1 X 0.375 Y-.375 F9. G41 D01 ( Ramp in start position cutter comp on )

G3 X.75 Y.000 R.375 Z- .4911 F 5. ( G code for climb mill )

G3 X .75 Y.000 I- .75 Z- .4196 ( Ramp in to cut point Circle mill )

G3 X.375 Y.375 I-.375 Z-.4107 ( Ramp out )

G0 X.0000Y.0000 G 40 ( Return to center X0Y0 point cancel comp. )

G0Z1.000 ( Retract from part )

[metalmayhem]

This is how you would use and program a ( 1 ) pass thread mill

not how I would do it when hand coding !
Aside from not throwing in a d comp or a given thread specifics - what I quickly jotted is pretty much how I do a single pass

[mountaindew]

he only aspect you should look out for is the feed rate. While the cutting takes place around the outside diameter of the thread, the center of the cutter only rotates on a very small circular path inside the hole (think of a .18" peg rattling inside a .25" hole, the center of the peg will rotate around a circle .25"-.18" = .07"). The cutting feed rate, as seen at the outside diameter will therefore be much higher than the feed rate programmed for the tool path. PathPilot Conversational automatically drops the actual programmed feed rate to compensate for this. If you pause the PP simulation while the thread is being cut you will see that the actual feed rate is much lower than the feed initially set in the conversational field. It can obviously also be seen in the G-Code. Fusion doesn't compensate automatically so you will have to adjust the Cutting Feedrate accordingly.
Step

I sent Tormach a Haas video explaining this in detail a while back. I was hoping they would pass it on to sprutcam to add a setting to mitigate this. The problem shows up in a big way on more then just thread milling As the haas video says at the start "you can hear it"

[mactec54]

not how I would do it when hand coding !
Aside from not throwing in a d comp or a given thread specifics - what I quickly jotted is pretty much how I do a single pass

It is best to add comp for a single pass as you almost always have to adjust, nobody uses a G91 for this operation, you did not include an arc on off which you need for it to work and yes It is easy to hand code for this simple program

[TurboStep]

Maybe I was not clear as to what I wanted to know . I was thinking of the thread mills that are similar to a tap . Move to the bottom of the, hole feed to thread depth , make one revolution , feed to center then out .

With respect, I still don't think you've asked what you really want to know. My very first response answered your first question with a yes, but perhaps you wanted to know how to set it up in PathPilot conversational?

vmax549 essentially got it right. Here's a screenshot with PP setup for a 1/4-20 multi-profile thread mill with a cutting diameter of 0.18"
https://www.lakeshorecarbide.com/14-...-uncoated.aspx



Z End is the bottom of the thread (-0.300") and Z Start is equal to Z End plus the thread pitch (-0.300 +0.050). In the example I've lifted Z Start by an additional 10% of the pitch for slightly more than one revolution to allow the spiral paths to overlap slightly.
This gives: -0.300 +0.050 +0.005 = -0.245"

PathPilot conversational only appears to allow threading from the top-down (conventional milling) whereas bottom-up (climb milling) is generally preferred. Disclaimer - I don't own any inch thread mills so I haven't run this example.

I used the Feed and Speed Suggestion feature form PP and I just noticed the suggested spindle speed is far too low for 6061. I'd use about 5000 RPM on my 1100.

... I'm not sure they understood the difference between a real thread mill, and single point thread mills which can have a different number of cutting edges but is still a single point cutter it appears there conversational programming is only for single point threading...

Uhh what? Just for the record selection or my "real" thread mills:



From the top: M2, M3, M4, M5, M6, M8 and 1/4 BSPT. I can assure you they are ALL "real* full profile thread mills, not the simple triangular tooth form found on common single point thread mills or similar Chinese thread mills. The same is true for my M1 x 0.25mm mill:



The smaller thread mills have only two rows of 3 teeth, as opposed to around 12-15 rows for the full depth thread mills, and I use them as though they were single point thread mills.
Step

[metalmayhem]

It is best to add comp for a single pass as you almost always have to adjust, nobody uses a G91 for this operation, you did not include an arc on off which you need for it to work and yes It is easy to hand code for this simple program

Like I said it was a quick jot that can easily be modified to suit whats needed , including adding d comp which is an absolute given . I've not found an arc in arc off to be necessary , but in my opinion more than one pass is in order to ensure a good clean thread