Thread milling when the hole is longer than the tool

[catfishearl]

I’m brand new at thread milling. I need to thread a 3/4-14 NPSM — 1.125 deep but my choice of tools are a .435 long insert or a .830 long insert.
How do I program the tool to go to 1.125 and climb up to Z0?

 

[Booze Daily]

Make your first helix at the bottom of the hole, then come up 4 or 5 pitches in Z and mill another helix.

 

[13engines]

Hey Catfish,

You can thread to any length as long as your tool has the needed shank length and clearance above the cutting edge. You just let your program go around more than once while continually rising. (or falling as the case may be)

So once you're past your lead in move where you're turning on comp, you simply allow as many full 3 axis circular moves as needed for the full length of thread, then start you lead out move while removing comp and you're done. You'll be double cutting a bunch of the thread length, but I don't think that's a problem. Not sure that you can machine full insert length, retract the Z height to match most the insert length, (but definitely some derivative of the pitch height, and then machine another full length. Someone may correct me on that. If your machine is accurate enough this may be the way to go too.

Hope this helps and/or makes sense to you. Good luck.
Dave

 

[catfishearl]

So, Z-1,125 then Z-.768?

 

[catfishearl]

I’m still a bit foggy on making the tool climb. Do I put a Z .0714 in each line ?

 

[13engines]

IF that is the lead length of your thread and you're machining in incremental mode... then yes. To be more specific, if your machine can do a full circle from a single line of code, then the above is true. If you need two lines for a circle, then cut your pitch height (Z move) in half on each line.

 

[Finegrain]

I’m still a bit foggy on making the tool climb. Do I put a Z .0714 in each line ?

You need to program 3D G2/G3's, assuming your control can helix in 3 dimensions.

You can also program a zillion G1's, but that is not feasible to do by hand.

Regards.

Mike

 

[angelw]

I’m still a bit foggy on making the tool climb. Do I put a Z .0714 in each line ?

Hello catfishearl,
The idea of using a Multi Pitch Thread Milling Tool is that a Thread Length within the length of the tool can be machined with one complete circuit of the Thread periphery with the tool. The alternative is to use a single point Threading Tool and make as many circuits to complete the Thread.

When the Thread is Longer than the cutting edge of the Thread Milling Tool, your alternatives are:

1. Cut the multiple pitches of the thread to the extent available with the length of the Thread Milling tool and then continue as if the Tool is a Single Point tool, making as many circuits as required to complete the Thread.

2. As Booze Daily suggests:
a. make one circuit with the Thread Mill
b. disengage with the Thread, re-position the tool and repeat the process of point a. above.

The disadvantage of method 1. is that the most parts of the Thread Cut in the first circuit of the Thread Mill will be subsequently repeatedly re-cut, possibly resulting in the Thread being loose in the area that is re-cut.

In Terms of Cycle Time, Booze Daily's suggestion would also be preferable.

Regards,

Bill

 

[toolsteel]

I use cam software to do this.....so my practical experience is less than many....
I agree with the method described by angel for hand programming.
I also seem to recall at one point some of the manufacturers of thread mills had programs / macro programs available free of charge for those hand programming.....i may have diremembered that ....it seems to happen.
I would take a look at the Vargus website first.....i believe they even have a phone app if you are into that sort of thing

 

[Hazzert]

Most threadmill manufactures have generators on their websites that'll do the code for you. Write some code and find one to compare.

 

[Rick Finsta]

I do this for an oddball ACME-like thread we're cutting at work. Just program a helix upwards from the bottom as many thread pitch multiples as it takes to reach the top. I post mine out of CAM.

 

[catfishearl]

With an insert .830 long how do I climb out of this to Z0?
G1G91Z-1.125
G1G41X.105Y.105D26F1.5
G3X-.105Y.105Z.0714I0J-.105F1.5
G3X-.105Y-.105Z.0089I0J-.105F1.5
G1G40X0Y0F30
G0Z.2
G90

 

[Booze Daily]

You don't need to climb out to Z0. You only need to climb out to shallower than Z-.830.

G0 X0 Y0
Z.1
G1 Z-1.125 F50.
G41 D1 X.375 F2.
G3 Z-1.0536 I-.375 (first helix up 1 pitch .0714)
G1 G40 X0 Y0
G0 Z-.6252 ( up 6 pitches in Z from where your last helix ended)
G1 G41 D1 X.375
G3 Z-.5538 I-.375 (second helix - you're less than Z-.830 so your insert is clear of Z0)
G1 G40 X0 Y0
G0 Z.2

BTW your code is not right. Don't program in incremental, you'll get yourself all confused.

G1G91Z-1.125
G1G41X.105Y.105D26F1.5
G3X-.105Y.105Z.0714I0J-.105F1.5
G3X-.105Y-.105Z.0089I0J-.105F1.5
G1G40X0Y0F30 (this move does nothing)
G0Z.2 (you just rapided up thru the side of your hole)
G90

 

[angelw]

With an insert .830 long how do I climb out of this to Z0?
G1G91Z-1.125
G1G41X.105Y.105D26F1.5
G3X-.105Y.105Z.0714I0J-.105F1.5
G3X-.105Y-.105Z.0089I0J-.105F1.5
G1G40X0Y0F30
G0Z.2
G90

Hello catfishearl,
Your above example will not work at all. You have specified Incremental Mode with the G1G91Z-1.125 Block. In Incremental Mode G3X-.105Y.105Z.0714I0J-.105F1.5 will move through the First Quadrant only; in which case the the J address is incorrect. The G3X-.105Y-.105Z.0089I0J-.105F1.5 Block will move through the Second Quadrant only. In both cases the Z value is incorrect.

Following is an example using Incremental Mode.

G90 G00 G54 X0.0000 Y0.0000
G43 Z0.5 H_ _
G01 Z0.040 F40.0
G01 Z-1.125
G91 G01 X0.0000 Y0.1250 F7.0
G41 G01 X0.4000 Y0.0
G03 X-0.4000 Y0.4000 I-0.4000 J0.0000
G03 X0.0000 Y0.0000 Z0.0714 I0.0000 J-0.5250
G03 X-0.4000 Y-0.4000 I0.0000 J-0.4000
G40 G01 X0.4000 Y0.0
G01 X0.0000 Y-0.1250
(2ND SECTION OF THREAD STARTS HERE)
G01 Z0.5712 F40.0
G01 X0.0000 Y0.1250 F7.0
G41 G01 X0.4000 Y0.0
G03 X-0.4000 Y0.4000 I-0.4000 J0.0000
G03 X0.0000 Y0.0000 Z0.0714 I0.0000 J-0.5250
G03 X-0.4000 Y-0.4000 I0.0000 J-0.4000
G40 G01 X0.4000 Y0.0
G01 X0.0000 Y-0.1250
G90 G00 Z0.5

In theory, the ramp in and out, circular moves in the Blocks shown in Red should have a portion of the Thread Lead specified, but in practice in doesn't cause a problem (Thread Form specific).

Hello BD,
Sorry about cutting across your answer; you Posted whilst I was typing.

Regards,

Bill

 

[catfishearl]

Booze and Angel! Thanks a million brothers! After almost 40 yrs of lathes, Swiss machines , gear shapers and Hobbs, surface and OD grinders I was dreading learning CNC milling at this stage. HOWEVER! You guys are getting me excited to be adding this machine family. The thread milling programs I’d looked at were all programmed in incremental. Thank God I don’t HAVE to use it. The whole G90/G91 thing was giving me brain cancer.

 

[acncguy]

Make your first helix at the bottom of the hole, then come up 4 or 5 pitches in Z and mill another helix.

...And all the online thread mill program generators I've used online take the first helix at the bottom of the hole, however, when using thread mills with inserts having multiple teeth, I’ve had problems taking the first helix at the bottom of the hole if the length of the insert used on the 2nd pass is considerably less than the full insert length cut that would be used at the bottom. You could find the bottom of the hole cuts smaller than the top. Also, chatter is more likely when plunging in with the full length of the insert, especially if not arcing into the cut. Of course, this varies depending on material, tool setup, type of tool, etc and can be remedied by adding passes, editing speeds/feeds, etc.

I suggest you even out the cut length used on the insert by taking the first pass as close to halfway down the thread length as possible, then the second helix at the bottom of the hole. Depending on the length of thread, this may need to be done 3 or 4 times; whatever is necessary. The percentage of insert length that would work without problems will vary by application.

You could program something like so:

(.540 diameter cutter cutting 3/4”-14 thread X 1.125" deep):

G90
G54X0.0000Y0.0000B0.000
G43Z.1000H1
G1Z-.5627
G91
G1G41X.0525Y.0525D1F10.0M8
G3X-.0525Y.0525Z.0089I-.0525J0.0000F1.5
G3X0.0000Y0.0000Z.0714I0.0000J-.1050
G3X-.0525Y-.0525Z.0089I0.0000J-.0525
G1G40X.0525Y-.0525F10.0M9
G90
Z-1.1339F50.0
G91
G1G41X.0525Y.0525D1F10.0M8
G3X-.0525Y.0525Z.0089I-.0525J0.0000F1.5
G3X0.0000Y0.0000Z.0714I0.0000J-.1050
G3X-.0525Y-.0525Z.0089I0.0000J-.0525
G1G40X.0525Y-.0525F10.0M9
G90
G0Z.1000


Regards,

Paul

 

[Spruewell]

If you are going to thread-mill several holes, you can program the path in incremental once, make it a sub-routine and save yourself a lot of typing.
It also makes tweaking and edits way easier when you only have to modify one part of your program.

 

[john-san]

I agree with many replies on this topic, and writing it in incrementallywill help significantly if you have more than just a few holes as spruewell suggests or using a macro .....he must be a moldmaker with that name?
I'm very curious what type of machine you have, since many over the last 20 or so years have canned cycles for helical interpolation built into the control
(Fanuc G36 CCW), allowing you to do it in one line. I'd have to confirm with one of our controls people, but that works the easiest.
I passed over a few comments, but just above me acncguy posted a G54 with a B0......are you using a rotary table or is this on a horizontal? One more thing, you're saying the inserts are .435 and .830 long....is that length/depth of cut?

I wouldn't want to take multiple passes, just start at the depth I need and go up past Z0, dont stop at Z0....thats a problem.