Thread Milling

[Anonymous]

IPA = India Pale Ale

I've done a quick air cut this evening, on an internal thread of 1mm pitch and 100mm diameter. With a feedrate of 100mm/min the cut cut took about 3 minutes. Ergo, the feedrate seems to be applied using the distance around the spiral, not that on the Z axis.

Regards,

Andrew

[richardandtracyParticipant @richardandtracy]

These are somewhat surprising tools. Is there really no UK source for them?

Regards,

Richard.

[Anonymous]

Posted by Richard Williams 7 on 25/06/2013 12:49:07:

These are somewhat surprising tools. Is there really no UK source for them?

Why? Feel free to add a link to a UK source.

Andrew

[John Stevenson 1Participant @johnstevenson1]

You can also use a tap with all but one flute ground off.

One pitch cuts all if it fits into the hole.

[Clive HartlandParticipant @clivehartland94829]

Got a Cromwell catalogue today that lists Thread Milling cutters, metric and pipe and other British threads. The prices , well, they are special!

Several bargains also appear in the milling cutter part.

I am not associated with Cromwell.

Clive

[Sub MandrelParticipant @submandrel]

Hi Clive,

How do you get hold of a paper Cromwell catalogue (I can get one through work if they are trade only).

Neil

 

>edit< Cancel that I just saw the big picture of a catalogue with 'request a catalogue' written by it!

Edited By Stub Mandrel on 02/07/2013 20:37:01

[John Stevenson 1Participant @johnstevenson1]

Neil, you could have had mine before I dumped it.

Never seen anything in there I can't buy cheaper or better from other suppliers.

Just been looking at broaches and they don't do the one I want but take say an 8mm keyway broach.

From Cromwell it's £244.81 and you need to push this thru 4 times with 3 added shims to reach depth.

They do a cheaper on at £119.48 but this one takes 6 passes to do the same job

J&L sell DuMont broaches which only require 3 passes [ big difference if you have a stick of gears to do ] for £79.50

No contest.

[John Stevenson 1Participant @johnstevenson1]

To get back to thread milling if you are doing an OD thread or biggish infernal thread you can use a Coventry die insert in a holder.

Same holder can be used to screwcut infernal threads on the lathe.

There's cheap and there's clever.

[Clive HartlandParticipant @clivehartland94829]

Luckily I have a Cromwell outlet very near my workplace and call in about once a month just to pick up the monthly cut price catalogue. They are selling 2 flute and 3 flute and 4 flute center cutting Carbide milling cutters in a set of 6 at a time for £29 or so. Rippa cutters also are reasonable in sets of 3. It takes me a couple of hours to read through and digest the contents and find the bargains. Agreed there are some expensive tooling in the catalogue but it is all named tooling like Ghuring and Mitsubishi. Just now and again I catch sight of bargains that are worth looking at further.

Clive

[richardandtracyParticipant @richardandtracy]

Interesting John. Not good for the tiny sizes I need, but looks good.

Is there any problem with the thread form when using thread milling with rapid helix threads?

The sort of thing I want to try to do is M13.5 x 3, triple start. In theory it's simple on my lathe. In practice, since I'm missing one of the gears for 3mm threading, it's less easy. Warco didn't supply the 63 tooth gear when I got it, and supplied me with a third 27 tooth instead. However, as it was 8 years before I noticed , I can't complain . Also, acrylic seems to be less easy than metals to thread & get a reasonable finish – you seem to have to go at either almost no speed or very, very high speed. I suspect thread milling will be more successful as the cutter speed will be very high on a tiny cutter.

Regards,

Richard

[John Stevenson 1Participant @johnstevenson1]

Richard,

Can't see a problem with that but you would need a single point tool as against the multi tools.

Pick up on the second pass will be interesting in that you will need to start 120 degrees away and 1/P down

Dont know what Warco lathe you have but ARC are selling some 63t gears to go with Neil's article in MEW 204

These are 1 Mod and have on OD of 65 mm to give you an idea of size.

Sent from my iPram

[BowberParticipant @bowber]

Late entry to the discussion I know but…

I've used the cutters shown by the original poster for a few years, they work very well and I've done smallish threads, twin start M6, and large threads, M16 + using two different sizes of cutter. All have been external threads though.

All my threads were coded using the NF wizard available in Mach3.

Steve

[Anonymous]

Steve: Thanks for the information; it's always useful to know that some-one has successfully used the tools. At least if I foul it up I'll know it's a defective operator, not the tooling. What sort of speeds and feeds did you use? Does the NF wizard come with Mach3 or is it a purchased add-on?

Regards,

Andrew

[BowberParticipant @bowber]

The NF wizards are included but don't work until you purchase a code. Not sure if there isn't a thread milling wizard in the normal wizards.

Just checked and there is a thread milling option in the normal wizards. I seem to remember that the NF one worked better though.

I think I just used a sensible speed, probably 75 – 100 mm/min but I can't remember. I tend to use slower speeds and work up but as I tend to do one offs I forget for next time

Steve

[John Stevenson 1Participant @johnstevenson1]

Careful with the thread milling wizards in mach there are bugs.

I have been repeatedly reporting them for about 5 or 6 years with no success. I'm told they work OK but even when i sent the files they are ignored.

 

Problem is Ron Ginger who is responsible for the wizards is American and only uses imperial. However like most Americans who think that Neil Armstrong was the first American to go abroad they can't accept that the rest of the world use metric.

 

Try this in the wizards.

 

 

Select metric, conventional, multi pitched cutter, right hand, inside.

 

Then do preview.

 

 

Always wanted to thread mill a D shaped hole

 

Imperial works fine. However when mach 4 comes out you won't even be able to do this as multi pitched cutters have been left out.

And I though Mach 4 was going to be aimed at industry ??

Edited By John Stevenson on 28/08/2013 21:41:32

[BowberParticipant @bowber]

Ahh, the mythical self locking thread is finally found!

[Sub MandrelParticipant @submandrel]

Can you input the metric measurements, pretending they are in Imperial and use a scaling factor of 25.4 for the output?

Neil

[John Stevenson 1Participant @johnstevenson1]

Possibly but why don't they fix the damn thing ?

Been broken from day one but as the guy concerned doesn't use metric the problem doesn't exist.

N I H syndrome.

Not Invented Here.

[Marcus BowmanParticipant @marcusbowman28936]

As far as I understand, if you are moving "normally" in X, Y and/or Z the same feed rate applies to the movement of the CP within that co-ordinate space. I think that means that if you are moving anywhere in X, Y or Z (including at an angle in two or three of those axes simultaneously) movement occurs at the feedrate set by the F command.

There is only one F command, so it is applied to X and/or Y and/or Z and any combination of those.

If you are using one of the other feed rate modes like inverse time mode, I believe different rules apply.

The more interesting question is how well does the control software cope with acceleration and decelleration while thread cutting? A first guess would be that it copes fine. A caveat is that some CNC-cut threads seem stiffer in the mating thread than they should be, and although this might be because the depth of cut is not adequate, the feel of the thread suggests the depth is fine and it is a problem with the approximations.

Marcus

[BowberParticipant @bowber]

Quite possibly Marcus, however the threads I've done have had a consistant feel to them.

I tend to cut them slightly large and try the nut and then adjust the settings so I get a nice fit.
The exception being an M6 twin start which fitted straight off.

Steve

[Anonymous]

Hmmmm, looks like I'm going to be writing my own G-code for thread milling.

I asked about feedrates for two reasons. One I'm interested to know what people use, so that I don't waste time cutting too slow, or badger the tool because I'm cutting too fast. The second reason is to do with how the control system interprets the F modifier. Logically the rate should be based on the distance of the vector sum of the move, ie, movement of tool CP, as described by Marcus. That's fine, and simple to calculate for G01 moves. But the sums get a bit more involved for G02 and G03. As far as I can see on my CNC mill the toolpath is correctly taken into account even when using G02/G03 for helical interpolation. A supplementary question is what happens when the A axis is in play? I'll need to experiment with this, as I am in the process of designing a two start worm, which will be milled using the 4th axis. If I ask the tool to move 100mm in X, and 10 revolutions in A, at a feedate of 100mm/min, is the move completed in 1 minute? The problem here is that the actual cutting speed of the tool will depend on the diameter of the workpiece, which the G-code does not explicitly know.

For threadmilling at the sort of feedrates that have been discussed I can't imagine the acceleration errors will be significant.

Regards,

Andrew

[Anonymous]

I think I now understand feedrates when using the 4th axis, at least in my version of Mach3. Mostly a case of RTFM!

For a move using only a rotational axis the F value is taken to mean degrees/min. So the following code:

G01 A360 F360

will move the 4th axis one complete rotation in 1 minute.

When a rectilinear axis is also involved in a move then the controller interprets the F value as inches/mm per minute. Of course for this to make sense the controller needs to know the diameter of the work. Funnily enough there's a box on screen so that one can enter a correction radius. Starting at X=Y=A=0 I entered the following code, along with a correction radius of 15mm, ie, diameter of 30mm:

G01 X-50 A1800 F100 all units in mm

The rotary axis made one rotation in a tad over 20 seconds, which is just about bang on for a feedrate of 100mm/min on work 30mm in diameter.

I've learnt something useful today, so I can tick that box, relax and grab a beer.

Regards,

Andrew

[richardandtracyParticipant @richardandtracy]

I have written two programs to get over the metric problem of the Mach 3 macros and also to permit the thread start angle relative to the X axis to be specified. I wrote the programs for myself, aiming them at a single point cutter with right hand threads on the XY plane. They may be usable by other people. You can specify multi start threads too. They come in two programs, one for internal & one for external threads.

If you go to my website here: **LINK** and select the first program in the list of downloads (CNC Thread Milling), you'll come across a page that explains the two programs and allows their download.

I hope they prove to be useful to someone.

Edited to say: if you have any problems or suggestions about the programs, please let me know.

Regards,

Richard

Edited By Richard Williams 7 on 12/09/2013 14:10:47

[richardandtracyParticipant @richardandtracy]

If anyone downloaded the thread mill programs I mentioned above, can I warn you of a program error, and suggest two interim work arounds.

Error: I have discovered a rounding error that occasionally makes the thread 1 pitch too long.

Interim work around: There are two interim work arounds, both work. 1) Inspect the g code in the program editor, check to see if the Z value is below the depth of thread expected and if it is, delete the last G2 instruction for each thread start. 2) Add an insignificant number to the thread pitch, 4mm pitch gives the rounding error, 4.0000000001mm does not, and when rounded to 5 decimal places it gives the same result.

Full fix: I shall try to correct the error today and post a new version of the programs to download by tomorrow morning.

Regards,

Richard.

[richardandtracyParticipant @richardandtracy]

Update complete.

I have also added a little program to create a toolpath to machine lithophanes from any bitmap image, too. The 'Heightmap Generator' plugin in CamBam was a little erratic & if I'd not checked the code produced, then I would have ended up machining the bed of my CNC machine. I found I was having to edit the toolpath for every new lithophane, which was tedious.

The Lithophane Generator I've written shouldn't need any editing, and because it uses rapid feed over blank areas of the picture, can be quicker than the output from CamBam.

I've used the program to create a 9" x 5.5" Lithophane, and the gentleman who received it was cock-a-hoop because it was such an unusual present. Anyone with a cnc mill, some machining time, and a bit of translucent Perspex can create one, only having to buy a £5 for 2 ball nose 2mm diameter end mill (dare I say, from China?). Link for these programs:

**LINK**

If anybody is interested, I have also written a program to take a G Code file and convert all arcs into short straight lines. This is a first step before producing a wrapper program. I had thought the wrapper program was complete, but discovered a few bugs that I'm fixing at the moment, and they are taking longer than I had anticipated. Ah well.

Regards,

Richard.

[Author]

Posts