Hello Guest it is March 28, 2024, 07:39:56 AM

Author Topic: Metric thread on inch machine?  (Read 7847 times)

0 Members and 1 Guest are viewing this topic.

Offline Chief

*
  •  16 16
    • View Profile
Metric thread on inch machine?
« on: July 14, 2011, 10:37:14 AM »
Hi Folks,

   Pretty much a beginner asking, so it it's especially dumb, please be kind :D
I want to do a metric thread mill on a Tormach 1100 set up for inch operations, but when I go to the NFW for thread milling (V286) it will not allow me to select MM instead of inch?
I can set the tool to MM, but if I continue into the wizard a pop up tells me it is converting the metric tool to inch?

Am I doing something wrong, or can I just not do MM threads on an inch setup?
Thanks
Terry

andrewm

*
Re: Metric thread on inch machine?
« Reply #1 on: July 14, 2011, 01:05:14 PM »
On the very first page at the top there is a option for MM or INCH, are you selecting that one before you move on to the next page?

I just posted a MM code for thread milling to mach, so it does work ^_^
« Last Edit: July 14, 2011, 01:08:15 PM by AndrewM »

Offline Chief

*
  •  16 16
    • View Profile
Re: Metric thread on inch machine?
« Reply #2 on: July 14, 2011, 01:38:57 PM »
Andrew,

  You nailed it! I was completly overlooking that selection, I'm so used to just selecting material there and moving on.  I was trying to do it on the page that shows all the tool data, it has LEDs for Inch/MM at the top and I was trying to select it there, even though there is no button, just clicking on the LED.

I just tried it and it works fine, after you got my brain properly calibrated!
Thanks
Terry

Offline Chief

*
  •  16 16
    • View Profile
Re: Metric thread on inch machine?
« Reply #3 on: July 15, 2011, 11:43:11 AM »
Andrew, everyone,

   I guess I spoke too soon when I said it worked fine, the setting up for metric worked fine, but  then I ran into trouble.
Again this is a Tormach 1100 mill using the Tormach supplied version of MACH 3.
Every time I set up to mill a thread it gives a warning that it is going to rapid Z to a number that is always = to what I program for depth, and then when I air cut the tool path just doesn't look right.  I am including below the code the NFW generated for an example cut.
The set up is for Al, using a .75" 10 tooth double bevel cutter.  I set it for a 2.0" minor diameter for 16 threads per inch to a depth of 0.5".  In the example it is only one pass, and is conv milling for an outside thread.
Besides the rapid Z move I don't understand, I don't get the other Zs moves up to about 2", I don't know if this is because the minor diameter is set to 2" or if it is a coincidence?
Any help someone could provide would be most appreciated.
Terry


(Code by Newfangled Wizard, 7/15/2011)
(Version 2.86)
(Program Posted for Aluminum )
G0 G49 G40.1 G17
G80 G50 G90 G98 
G20 (Inch)
(***** Thread Milling *****)
M6 T7
M03 S2546.5
M9
G00G43 H7 Z2
(Right Hand OD Conv)
(WARNING THis is going To RAPID down to Z-0.5)
X1.75 Y0
G00 Z-0.5
G01 X1.375 F47.3
G03 X-1.375 Y0 R1.375 Z-0.4688
G03 X1.375 Y0 R1.375 Z-0.4375
G03 X-1.375 Y0 R1.375 Z-0.4063
G03 X1.375 Y0 R1.375 Z-0.375
G03 X-1.375 Y0 R1.375 Z-0.3438
G03 X1.375 Y0 R1.375 Z-0.3125
G03 X-1.375 Y0 R1.375 Z-0.2813
G03 X1.375 Y0 R1.375 Z-0.25
G03 X-1.375 Y0 R1.375 Z-0.2188
G03 X1.375 Y0 R1.375 Z-0.1875
G03 X-1.375 Y0 R1.375 Z-0.1563
G03 X1.375 Y0 R1.375 Z-0.125
G03 X-1.375 Y0 R1.375 Z-0.0938
G03 X1.375 Y0 R1.375 Z-0.0625
G03 X-1.375 Y0 R1.375 Z-0.0313
G03 X1.375 Y0 R1.375 Z0
G03 X-1.375 Y0 R1.375 Z0.0313
G03 X1.375 Y0 R1.375 Z0.0625
G03 X-1.375 Y0 R1.375 Z0.0938
G03 X1.375 Y0 R1.375 Z0.125
G03 X-1.375 Y0 R1.375 Z0.1563
G03 X1.375 Y0 R1.375 Z0.1875
G03 X-1.375 Y0 R1.375 Z0.2188
G03 X1.375 Y0 R1.375 Z0.25
G03 X-1.375 Y0 R1.375 Z0.2813
G03 X1.375 Y0 R1.375 Z0.3125
G03 X-1.375 Y0 R1.375 Z0.3438
G03 X1.375 Y0 R1.375 Z0.375
G03 X-1.375 Y0 R1.375 Z0.4063
G03 X1.375 Y0 R1.375 Z0.4375
G03 X-1.375 Y0 R1.375 Z0.4688
G03 X1.375 Y0 R1.375 Z0.5
G03 X-1.375 Y0 R1.375 Z0.5313
G03 X1.375 Y0 R1.375 Z0.5625
G03 X-1.375 Y0 R1.375 Z0.5938
G03 X1.375 Y0 R1.375 Z0.625
G03 X-1.375 Y0 R1.375 Z0.6563
G03 X1.375 Y0 R1.375 Z0.6875
G03 X-1.375 Y0 R1.375 Z0.7188
G03 X1.375 Y0 R1.375 Z0.75
G03 X-1.375 Y0 R1.375 Z0.7813
G03 X1.375 Y0 R1.375 Z0.8125
G03 X-1.375 Y0 R1.375 Z0.8438
G03 X1.375 Y0 R1.375 Z0.875
G03 X-1.375 Y0 R1.375 Z0.9063
G03 X1.375 Y0 R1.375 Z0.9375
G03 X-1.375 Y0 R1.375 Z0.9688
G03 X1.375 Y0 R1.375 Z1
G03 X-1.375 Y0 R1.375 Z1.0313
G03 X1.375 Y0 R1.375 Z1.0625
G03 X-1.375 Y0 R1.375 Z1.0938
G03 X1.375 Y0 R1.375 Z1.125
G03 X-1.375 Y0 R1.375 Z1.1563
G03 X1.375 Y0 R1.375 Z1.1875
G03 X-1.375 Y0 R1.375 Z1.2188
G03 X1.375 Y0 R1.375 Z1.25
G03 X-1.375 Y0 R1.375 Z1.2813
G03 X1.375 Y0 R1.375 Z1.3125
G03 X-1.375 Y0 R1.375 Z1.3438
G03 X1.375 Y0 R1.375 Z1.375
G03 X-1.375 Y0 R1.375 Z1.4063
G03 X1.375 Y0 R1.375 Z1.4375
G03 X-1.375 Y0 R1.375 Z1.4688
G03 X1.375 Y0 R1.375 Z1.5
G03 X-1.375 Y0 R1.375 Z1.5313
G03 X1.375 Y0 R1.375 Z1.5625
G03 X-1.375 Y0 R1.375 Z1.5938
G03 X1.375 Y0 R1.375 Z1.625
G03 X-1.375 Y0 R1.375 Z1.6563
G03 X1.375 Y0 R1.375 Z1.6875
G03 X-1.375 Y0 R1.375 Z1.7188
G03 X1.375 Y0 R1.375 Z1.75
G03 X-1.375 Y0 R1.375 Z1.7813
G03 X1.375 Y0 R1.375 Z1.8125
G03 X-1.375 Y0 R1.375 Z1.8438
G03 X1.375 Y0 R1.375 Z1.875
G03 X-1.375 Y0 R1.375 Z1.9063
G03 X1.375 Y0 R1.375 Z1.9375
G03 X-1.375 Y0 R1.375 Z1.9688
G01 X-1.75
G00 Z2
M5 M9
M30

andrewm

*
Re: Metric thread on inch machine?
« Reply #4 on: July 15, 2011, 12:00:08 PM »
So is it overriding what you tell it to make the rapid? or are you not programming that?

Offline Chief

*
  •  16 16
    • View Profile
Re: Metric thread on inch machine?
« Reply #5 on: July 15, 2011, 12:38:33 PM »
Andrew,

  Correct, it is making the rapid without any input from me. I have not added (or subtracted) anything, everything in the example is from the wizard.
I should have added for the setup, that I referenced all on the machine then set zero x,y to the center of the material to  be threaded and z to 1" about that for the air cut.

I didn't run them but programing the same example in older versions of NFW (285 & 272) show the same rapid in the begining.
Terry
Re: Metric thread on inch machine?
« Reply #6 on: July 15, 2011, 01:06:50 PM »
This is going to cut from the bottom of the cut upward. Hence the rapid move to Z -.5

then it move in to the right cutting depth (X 1.375) This is 1" for the minor dia or 2" and .375 for half the .75 cutter dia.

The cut above 0 is caused by the Rapid height box- you must have 2" in that.

I think the wizard would be better if it had a top of cut box, Now it cuts until it reaches the rapid height value.

I will see about fixing that.

andrewm

*
Re: Metric thread on inch machine?
« Reply #7 on: July 15, 2011, 01:22:25 PM »
Thanks Ron

Offline Chief

*
  •  16 16
    • View Profile
Re: Metric thread on inch machine?
« Reply #8 on: July 15, 2011, 01:32:08 PM »
All,

Ron is correct, (well Duh!) I ran the code in the example, except that I changed the rapid height to .1 and it did indeed rapid down and cut going bottom to top. And it does attempt to cut until it reaches the rapid height, so you definetly don't want to set that too high!

When I first got the mill I cut a thread on a dowel and I'm almost positive is went top to bottom, but that would have been with the old thread mill wizard, because it was before I bought the NFWs.

If you are interested in an opinion, I would definetly like to see the mod the Ron mentioned, top to bottom just seems more natural to me, on the other hand it works.

Thanks to all, especially Andrew and Ron, for helping me understand this.
Terr
Re: Metric thread on inch machine?
« Reply #9 on: July 15, 2011, 03:00:42 PM »
This takes a while to get your head around, but if you consider the options of climb or conventional, right hand or left hand, it is necessary to go both bottom to top and top to bottom.  Try changing to conv milling and it will go top to bottom.

I will add the top of cut DRO to my list for the next time I make a release.