Help with threading on a CNC mill

[shorety]

Hello all, I am a total newbie when it comes to mills so I'm banging my head on the table trying to figure out how to thread on a mill.

The machine I am using is a 1994 Supermax, Max 1 Rebel with a Fanuc O-M controller. I am using Bob-Cad for programming.

I have created the program and ran it on the mill but the program does'nt have any G codes related to threading like G33, G92, or G76. It also just runs 1 pass. I have read in the books we have here at the shop and also read through posts and from what I can tell there should be one of these in the program. I'm assuming that our mill, being an older model, wont be able to us the G76.

What I'm trying to do as a test is thread an I.D. hole to 1" - 8 TPI, 1" depth.
I also would like to know how to be able to run multiple passes to get to the finish depth.

If anyone has an example of what the program should look like or have any advice for me that would be great.

Thank You.

[Geof]

The threading cycles you mentioned are for a lathe not a mill. Threading on a mill is done by using helical interpoleation; the machine interpolates a circle using G03 or G02 and at the same time moves the Z axis.

It is possible your machine will not do helical interpolation; try something like:

G03 I0. J-.5 Z.1
G03 I0. J-.5 Z.2
G03 I0. J-.5 Z.3
G03 I0. J-.5 Z.4

and see if the Z axis moves up 0.1 at each circle.

[shorety]

Ok Geof, I tried that and it worked. Thank you.

So now if I use the G03 and just input in the distance of the treads along with feed rate I should be able to achieve the threads I am looking for?

Also is there a certain reason why Bob-Cad wrote the program the way it did? I made sure that it was not in lathe mode when I created the tool path for the spiral thread.

Thanks again.

[Geof]

Originally Posted by shorety Ok Geof, I tried that and it worked. Thank you. So now if I use the G03 and just input in the distance of the treads along with feed rate I should be able to achieve the threads I am looking for?...

There is a little more to it than that but that is the fundamental idea. Are you familiar with tool comp? What type of tool do you have, single point or a thread mill?

Do a search here on CNCzone and you should find several threads/posts about thread milling.

[shorety]

Sorry, I am not familiar with tool comp.

The tool we will be using is a thread mill.

[Geof]

The advantage to using a thread mill is you need only do one or two circles to finish a longish thread.

If you can convince Bob-Cad to output code that works then you don't need to worry so much about tool comp because you can tweak sizes in Bob-Cad. I don't use and Cad or Cam and with hand coding tool compensation makes it easy to adjust sizes. Also with tool comp it is fairly easy to take the thread in two or more cuts which for a coarse thread may be useful.

[PixMan]

Originally Posted by Geof The threading cycles you mentioned are for a lathe not a mill. Threading on a mill is done by using helical interpoleation; the machine interpolates a circle using G03 or G02 and at the same time moves the Z axis. It is possible your machine will not do helical interpolation; try something like: G03 I0. J-.5 Z.1 G03 I0. J-.5 Z.2 G03 I0. J-.5 Z.3 G03 I0. J-.5 Z.4 and see if the Z axis moves up 0.1 at each circle.

Good test other than he'll need to have a feed rate in there. Not sure if it'll need inches-per-minute or degrees per minute.

EDIT: Nevermind, I see you got it working.

Feedrate for thread milling is not like single-point threading on a lathe. Your Z-axis move within one rotation is your thread pitch. Feed only regulates the metal removal rate here. The example shown makes 10 threads per inch or per millimeter.

[Geof]

Originally Posted by PixMan Good test other than he'll need to have a feed rate in there.... ...The example shown makes 10 threads per inch or per millimeter.

The feedrate was on the G41 move to set tool compensation on a lne above that I omitted.

10 threads per millimeter would qualify as a fine thread; yes I was thinking in inches.

[SteveinAZ]

Shorety, if you want to hand code it, it's really pretty easy - the sample below is generated from Excel using a 0.620" diameter 4 flute thread mill, assuming you want 1.0" of good threads, 350sfm@0.003"/tooth chipload. The diameter you put in your control to start with can be 0 (zero) or so, and then you can adjust the thread diameter until you get gage perfect threads. For an 8 pitch, I would make two passes on the thread and enter two diameters in the control - that's a pretty deep thread (pitch wise) and a deep hole, so you will probably get a tapered thread if you tried to knock it out in one pass. So with this example, I have used tool 1, diameter 1 offset (set at 0.020 DIAMETER in the control) for the first pass, and the second pass will use diameter offset 41 (set at 0 diameter) [I usually use a cooresponding offset number that is tool number plus number of tools in the magazine, so in this case, I would enter 41 with a 40 tool chain]. Although this program will do a double Z move in and out of the hole between the first and second pass, it is easy for me to see that it always returns to the correct starting point before going into the hole the second time. If your threads are gaging small, you will need to change the diameter offset 41 in the negative direction, so you could end up at a diameter offset of -0.020" (that's actually a pretty common diameter for us).


T1M6
G17G40G90G64G80G98
G90G54G0X0Y0
S2156M03
G0G43H1Z0.100

G0G91Z-1.0156
G1G41X0.0950Y0.0950D1F19.66
G3X-0.0950Y0.0950Z0.0156I-0.0950J0F9.83
G3X0Y0Z0.1250I0J-0.1900F9.83
G3X-0.0950Y-0.0950Z0.0156I0J-0.0950F19.67
G1G40X0.0950Y-0.0950F30.0
G0Z0.8594
G90
Z0.100

G0G91Z-1.0156
G1G41X0.0950Y0.0950D41F19.66
G3X-0.0950Y0.0950Z0.0156I-0.0950J0F9.83
G3X0Y0Z0.1250I0J-0.1900F9.83
G3X-0.0950Y-0.0950Z0.0156I0J-0.0950F19.67
G1G40X0.0950Y-0.0950F30.0
G0Z0.8594
G90

Hope this helps.

Steve

[hpmachining]

Here is a link to some excel spreadsheets that help with thread milling:
http://www.micro100.com/downloads/ThreadMillAssist.html