I need the spindle not to turn, but the table needs to move per g-code

General Discussion
#1

I have an application where I need the spindle not to turn, but the table needs to move per g-code. Attached (using the 4 bolts in the spindle nose piece) to the spindle is a hi-speed 220 volt spindle with manual collet system, that I do not want for all the obvious reasons not to turn, for safety I plan to remove the “v” belts from the spindle to the motor.
Is there a way to remove all reference to the spindle g-code command after using BobCad to generate the tool path? I know when I program a part in BobCad I am given choice about speed & feed for the tool, but what if I need to have no reference to the spindle to come on.
The controller is Fanuc OM, around 1995, red cap AC drives. In the Fanuc parameter 24.2 = 1 now, I have changed to allow the controller not to see that the spindle is up to speed or not, so it will accept just the x. y, & z axis command and move the table, but must never see a spindle command.

I hope that I have given enough correct information that someone has done this before?

#2

Hi,
you can adjust your Post Processor deleting (commenting) all occurrences of ‘spindle_on’. To get sure also check, if there is no M3, M4, M03 and M04 hard coded in the PP.
Regards, Harald

1 Like
#3

MillingGuy, thank you! Are you suggesting that in BobCad v29 while creating the program that will be saved as a g-code file, that there is a way to delete the part referring to the spindle? This is NOT something that is done in Predator Editor?
I will study BobCad v29, the command/options that are available, what type of command am I looking for or what tab is it under?

Many thanks!!

#4

Hi,
for each Milling Job you define the machine to use therefore which PostProcessor should be used to generate the proper G-Code. In case of BC_3x_Mill machine it defaults to PostProcessor file BC_3x_Mill.BCPst
image

It is the *.BCPst file (just text information) where you can kick out the phrases mentioned in my first answer. You have to do the changes with your Fanuc PostProcessor.
I suggest to first make a copy of the file before doing the changes :wink:

Good luck, Harald

1 Like
#5

MillingGuy, thank you!!! I do not think I would have looked in that folder, I will try a new part in the morning, after reviewing the folder looking for *.BCPst file.

I was thinking in Predator Editor, using “find & replace” command.

Many thanks!

#6

Hi
sure you can do it in Predator or any Editor also. But you have to do it every time after generating the G-Code. Modifying the PP file all is done during the Post process.
Bye, Harald

1 Like
#7

MillingGuy, many thanks, you were correct, no “m” code are saved. Will this g-code that I have saved using the BC_3x _Mill.BCPst (post processor?) run as is, or does this need to be tweaked? This mill is new to me, I have not been able to get the table to move by g-code yet, that could be that the parameter that was changed to allow the table to move w/o the spindle coming up to speed, or it may be the post processor I was using.

I have received this suggestion to start the CNC G-code file with something like this:

N10 G90
N20 G10 P1 X-12.5000 Y-8.000 Z-12.0000 (P1 -Set the Datum of G54 )

G54 (G54 work offset active)

Here Your program goes
.
.
.
My hope is that I can use “zero return” when I start a new part, use the preset x=0, y=0 saved in the mill with the part in a vise with a stop (so all parts will use this same location), so I don’t need to find the start point for those 2 axis and z axis is the axis that does not have a toolholder, using collets, so I will need to set z axis every time the tool is changed, this is ok, I was aware of this.

Have I understood this correctly? I am open to suggestions.

Many thanks for your help!!

#8

I see a few m codes after close inspection, this is what I see, pics attached. Line 26, 27, 28 & 3477 have m code showing.

Postprocessor M05
Postprocessor M05486×975 66.5 KB

Postprocessor m code
Postprocessor m code505×568 36.1 KB

Many thanks!

#9

When a tool is to be changed, I will need a “tool change operation” to allow manual operation, install next tool & to “set” tool location (go to machine settings and get the correct offset data), go to tool offset screen (G53?) input the correct offset data and continue the program, is this close?

Do I need to use the BC_3x _Mill.BCPst (post processor?

It appears to me that the g-code will need to be stripped of the “M CODES” in Predator Editor, and save this, then add the tool change routine for each tool change, then save this to cut part. Am I getting close?

Many thanks!

#10

You might want to change the M05 to a M19 unless you do not need to stop your spindle from turning.

1 Like
#11

Eric, thanks!! It is not important that the spindle is stopped or freewheeling, the mount for the hi-speed spindle will not allow the BT-40 spindle to rotate when installed.
What is important is not have the motor to the BT-40 spindle get power, I will have belts off the spindle motor so if it starts it will not turn the spindle but will burn electric. The hi-speed spindle will be kind of permanent to the mill while I have it, all can be unbolted to remove.
Many thanks!!

Edit: I understand, M06 (Tool Change), M03 (Start Spindle Clockwise), & M04 are the only ones to worry about and remove. This may be closer to correct than I realized.
Many thanks!!

#12

I f you got a tool changer on the mill, you might want to delete the M06 too

1 Like
#13

PJK, many thanks, good thinking!! I will do that even though the air will be disconnected, my tool changer is the umbrella style, it uses air to move toward the spindle.
As to be clear, I used the “find (MO3, MO4, MO6) and replace=M05” in Predator Editor after the post processor change in BobCad, (as per MillingGuy’s suggestion).

From “MillingGuy” in earlier post M3, M4, and M03 and M04 are not the same and need to be search for as well, separately?

The is from my earlier post:
"I have received this suggestion to start the CNC G-code file with something like this:

N10 G90
N20 G10 P1 X-12.5000 Y-8.000 Z-12.0000 (P1 -Set the Datum of G54 )

G54 (G54 work offset active)

Here Your program goes
.
.
.
I understand that the “machine location” will be used with this suggestion shown above. I am looking for a way to make the path to get usable g-code to the mill with as few steps as possible. I need to understand what I can automate (not really) but make it as easy as I can for myself. I am searching for suggestions around this.

Many thanks

Edit: I have “machine motion” by command!! It ran for a while 15 minutes and received a Fanuc alarm 008 that says that a M02 M30 or M99 was needed in the program. Apparently too good of a job removing M0 from the program. I did not use the “check” button on the control, but will next time.
Many thanks!

#14

In Predator Editor, I have found the edit machine template (3AXVMILL); I unchecked the “Tool Change M6” and unchecked program numbers, to conserve memory in mill. This first attempt did not take out the M6 or program numbers (the numbers I want out are at the begging of each line, (line & block are 1 and the same, correct?))

The only way so far is to use 'find & replace = M5" using Predator Editor.

If there is a better way, now is the time to share the secret handshake!!

Many thanks!

#15

@metal2cut
I’m sorry, I can’t keep up with what you’re trying to do. Originally understood that your milling spindle should not rotate. In regular machines work like this:
M3/M03 … turn spindle clockwise
M4/M04 … turn spindel counterclockwise
M5/M05 … stop turning spindle
M6/M06 … insert new tool
M7/M07 … mist coolant on
M8/M08 … flood coolant on
M9/M09 … mist and flood coolant off

Finally, it is the postprocessor used that determines how the G-code is generated. So you have to find out which PP BobCAM uses in your case and adjust it so that no M3 or M4 (M03/M04) instruction is generated.

Regards, Harald

1 Like
#16

MillingGuy, thank you, I will need to edit the g code every time, or I need to “adjust it so that no M3 or M4 (M03/M04) instruction is generated.”

I read this, and it sounds like a special post processor for my situation would be the ideal solution. Did I read and understood this correctly? If so, is there any suggested reading I should look at? I will be using this set-up (the PP to remove spindle commands) for this ongoing application. I am interested in creating a new PP if this is possible and will speed and have a higher degree of safety & accuracy, hopefully the program will be ready w/o any more editing program manually. The mill is a bed mill style, with axis travel 25"x16"x24", no ATC.

Any help in, creating a post processor for this application would be warmly welcomed, many thanks!

#17

Hi,

upload the PP you are using. It is just a text file with extension *.BCPst. Then we can try to do the next step. You can find your used PP here:
image
Note: this is just an example, if I use BobCad default BC_3x_Mill machine that uses by default the BC_3x_Mill.BCPst postprocessor

Regards, Harald

#18

MillingGuy, From your earlier suggestion, I am using the “3AXVMILL PP” from the screen you show in the above thread. Then I would use Predator Editor to “find & replace” the MO3, MO4 & MO6 are replaced by MO5. This PP is the only PP that I have tried, and allowed the mill move, there could be other PP that will work, for example the FanucOM.BCPst is the only Fanuc PP listed. The controller is a 1995 (B) Fanuc OM. I am open to suggestions, if one PP is easier to tweak than the other.

This is the PP I used:
See next post for the proper Fanuc OM PP.

I think this has copied correctly, if not I will try again!
Many thanks!!

#19

@metal2cut my example was just an example. I do not know, what PP you are using, but you can figure it out going the way I did…

You have to sent/upload you PP file. BC_3x_Mill.BCPst is just one of many other PP files out there when you install BobCam. And BC_3x_Mill is a generic one from BC that can be used as a starting point if no other PP file do the job for ones machine.

Bye, Harald

#20

MillingGuy, many thanks!! I have a sample program that I used this PP with, and just ran it & it ran ok, just seems best to start with a PP that is best suited for the controller, PP is attached.
I will need to pause some programs to install the next tool, and “touch off” for the Z axis.
This is the PP, for Fanuc OM:
Fanuc0M.BCPst (27.2 KB)

Many, many thanks!