M5 instead of M3

[Lee.]

Hello All.

 

I am using a Fadal Post and on some tools it outputs an M5 instaed of an M3 for Spindle Start.

 

Does anyone have any ideas?

[gcode]

Check the tool definition and make sure its not set to counter clockwise

[Columbo™]

I only see this problem if there is "0" (zero) in the spindle speed box....

[Lee.]

I checked it and it is greyed out, but clockwise.

 

I thought CCW was M4

 

I'm getting an M5 which is spindle stop??

[Alvaro Gil - Cimquest-inc.com]

You sure you don't have a "0" zero for the spindle speed?

[Thad]

quote:

---

I thought CCW was M4

---

It is.

 

 

I'm with Alvaro, check the RPM.

 

Thad

[Lee.]

SS is set to 255 for a 3/8" RH Tap.

 

I am rigid tapping.

 

It outputs M5???

 

It's very strange.

[Lee.]

N160 G0 G17 G40 G80 G90

N170 ( 375-RH-TAP TOOL - 1 DIA. OFF. - 6 LEN. - 1 DIA - .375 )

N180 T1 M6

N190 G0 G90 S255.2 M5 M90 E1 X0. Y0.

N200 H1 Z.1

N210 G84.1 G99 X0. Y0. Z-1.04 R0.1 S255.2 F15.94

N220 G80

N230 M5

 

 

like this on line N190.

[G10X0Y0Z0]

if i remember correctly the spindle starts up at the g84.1. the reason mc is outputting a m5 is that the control needs to see the spindle stopped. run the program above the part and see if the machine starts up the spindle at the g84.1

i do believe your m90 s255.2 needs to be in the line just above the g84.1. it's been a long time since i worked on a fadal

[Tim Johnson]

Here's our tap on a Fadal;

code:

---

N1030(1/4-20 UNC-2B TAP RH)

N1040T6M06S800.2

N1050G90M05

N1060G84.2

N1070G00X3.3752Y-3.8401E1T7

N1080H6Z2.M08

N1090Z.4

N1100G84.1G99Z-.525R0.4S800.2F40.

N1110X6.3098Y-5.0529

N1120X6.9137

N1130X7.6304Y-5.0533

N1140X8.3177Y-5.0531

N1150X7.987Y-6.5864

N1160X7.7628Y-7.4445

N1170X9.5183Y-8.3197

N1180G00G80Z.4

N1190Z2.

N1200G91G28Z0M09

N1210M01

---

[d.park1]

Run fadals everyday,this should work for you.

 

 

N1 O1234 ( TAP )

N2 ( CREATED ON 08-01-08 AT 4:35 PM )

N3G20

N4G0G17G40G80G90

N5 ( 3/8-16 TAPRH TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA - .375 )

N6T1M6

N7G0G90S80.1M5M90E1X0.Y0.

N8H1Z1.M8

N9G84.2

N10G84.1G98X0.Y0.Z-.5R0.1S80.1F5.

N11G80

N12M5M9

N13G90H0Z0.

N14E0X0Y0

N15M30

[Thad]

I was going to ask if it was a tap, but I figured you'd have mentioned it if it was.

 

Fadal recommends NOT turning on the spindle (don't know why since it still works if you do) when tapping. The code below will work, although I don't know what M90 is. I've never used it and I've probably tapped over 1000 holes on Fadals. As others have mentioned, the G84.1 will take care of turning the spindle on.

 

code:

---

N160 G0 G17 G40 G80 G90

N170 ( 375-RH-TAP TOOL - 1 DIA. OFF. - 6 LEN. - 1 DIA - .375 )

N180 T1 M6

N190 G0 G90 M90 E1 X0. Y0. <-- NO S OR M5!

N200 H1 Z.1

N210 G84.1 G99 X0. Y0. Z-1.04 R0.1 S255.2 F15.94

N220 G80

N230 M5

---

Also, the ".2" in the RPM is only necessary when tapping above 750 RPM.

 

Thad

[Thad]

Just noticed you guys (Lee, Tim and d.park) must be running Format 2. Otherwise your F would be your RPM and your Q would be the pitch.

 

Thad

[Lee.]

Thad and All,

 

Yes I am running Format 2, It's easier for me to understand, being of Fanuc Based Programming for 9 years.

 

I will try it as posted in fresh air and let you know what I find.

 

I haven't run the machine much so am not very experienced in it.