Using 2 spindles to ruff & finish pockets & profiles. Fanuc OM, Supermax2 with mounting Z axis for 2 spindles, need help understanding machine offset

[solidworks4u]

Using 2 spindles to ruff & finish pockets & profiles in 1/8" aluminum plate. Fanuc OM, Supermax2 with mounting on Z axis for 2 spindles, need help understanding machine offset inside Fanuc OM controller and or BobCad v29.
I had success with single spindle and BobCad v29 even though the Post Processor is not perfect. I review each program for the -Z and edit out as to not allow the z axis to go all the way back to "home", (Z axis all the way up) location. By mounting 2 spindles about 9 7/8" (x direction) apart from each other. All the parts are small, all have at least 1 pocket & the profile needs a finish cutting on each part.
To set up, usually the part is against a stop, held in a vise, attached to a tool block with a 1/4" reamed hole to use as the same starting point no matter what the shape of the part is. Using a dial indicator, in the 1/4" reamed hole, to locate each spindle (ruff/finish or Left/Right) in relationship to the machine. It is as follows; Left spindle [X=-13.2410 & Y=-5.9523] & Right spindle [X=-23.1187 & Y=-5.9504].
I believe each of these sets of these dimensions will be used so the controller in the machine offset. In BobCad, I am not shore if there is a way to save any time or make more consistence or allow for fewer mistakes.
Every part has 2 programs, ruff pass will have an additional finish program that requires the operator to turn off or on the spindle to match the type of program to the part. If the cut time becomes short, I will keep the spindle running at low speed.

From earlier conversation with, I think it was Vancbiker does his programs using 2 spindles. I am still a newbie, with this controller. All suggestions are welcomed. Many thanks in advance.​

 

[Vancbiker]

I have 2 machines, not 2 spindles on one machine.

 

[solidworks4u]

Vanbicker, sorry, my mistake. Wish you well!

 

[Ox]

Is there a question posed?

I don't understand how you can possibly have a second X/Y offset?
I understand a second Z offset, but Spindle 2 would seem to be a slave?

I have only seen these mills in magazines.


-----------------

I am Ox and I approve this here post!

 

[macgyver]

I have a multi spindle router with an OM on it and I use it in two ways; if I am doing the same cut but with multiple spindles it is setup and ran like a duplicator so the extra spindles are slaved. This means the Master has the work coord, tool length and dia comp. I have to manually match the others to this one. I then change the program to call up all the spindles I want to run by the T number and that is the only code needed to slave them.

Otherwise I use them individually like a toolchanger and each spindle has it's own work coord, tool callout and tool length and dia comp.

Does your machine have a tool changer for each spindle?

 

[solidworks4u]

Ox & macgyver, many thanks. My hope is to use one spindle to ruff the part in, using a larger tool, then have the other spindle take a finish cut with a small tool.
After re-reading macgver's post, I plan to try 2 programs, use the work coord and tool length & diameter to match the ruff or finish requirements for each part.

There is no tool changer for the hi-speed spindles, using a 2nd spindle is the workaround, so fewer tool changes.
Many, many thanks!

Edit: By having 2 stand-alone programs a ruffing & a 2nd program to take finishing cut is the safest, my concern to have the next spindle on, ready with air & coolant before the cut starts. All of this is manually operated. My question if there was a better way to approach without ATC.

Many thanks!

 

[solidworks4u]

After pondering & praying, about how and what is required, as long as there are separate programs, 1 to ruff & a 2nd program to finish the tool will need a separate "offset" for each tool saved in the controller. This tool needs to be consistent in each of the programs and consistent to work coordinate. These are the work coordinates: [X=-13.2410 & Y=-5.9523] & Right spindle [X=-23.1187 & Y=-5.9504] that are set G54 & G55 to. Is there a standard approach to work coordinates?
My question; have I explained my approach well enough for others to follow? I need a 2nd opinion.

Many thanks in advance, all suggestions welcomed.

 

[Ox]

I for one have no clue how you have an x/y offset for a second spindle.
I would ass_u_me ot to be a slave.

So - maybe we are not looking at the same machine.
So - again - if you could post a pic of the machine so that we are all on the same page?

Otherwise, if you want to use 2 different offsets for the same tool, I think that you could just call up a different H value?
I am very green on Fanuc mills, but I would think that works?


---------------------

I am Ox and I approve this here post!

 

[solidworks4u]

Ox, thanks for your thoughts. This pic shows how the 2 spindles are mounted with blower, & filtered air manifold (the green part is cool air manifold) to the Z axis. The vise has a stop to locate a tooling block that a reamed 1/4" hole is known or X & Y = 0.0 of the part, or G54 left spindle or G55 is the right spindle. The coolant supply hose has not run yet, my thinking is a dedicated liquid coolant supply (if there is an issue about why no coolant, it will be easier to find) for each nozzle & just left / right air valving (turn off left; open right side for example) include the power supply to each spindle, may turn to lowers speed when not cutting with that spindle. I am thinking the safe approach is 2 programs (ruff & finish) for each part, but may find better to track the part if only a single program with a "pulse" to get the spindle & coolant correct. The air to cool the spindles is on all the time to both spindles & the manifold has rubber gaskets to each spindle.
I pray this helps to explain what I am working on.

 

[Ox]

Well I can see a carousel toolchanger for the left spindle.
Is there not one for the right spindle?

I take it that you have never ran this machine?


--------------------

I am Ox and I approve this here post!

 

[solidworks4u]

Ox, I know that this approach reduces the size of the part, but that is OK, my part is small size of a playing card. Earlier I had just a single hi-speed spindle mounted in the same machine & have cut parts. The ruffing tool will be around .062" diameter & the finish tool .032" diameter, max depth .125" in aluminum. I have had success with 6061-T6, but open to suggestions for alloy that cuts better, that is reasonable cost.

 

[Ox]

OK, I think I git what you are wanting to doo.
You doo NOT want to run 2 parts at the same time, but rather you are looking to rough on one spindle and shuttle the same part over to the 2nd spindle for a finish cut?

In this case - yeah, I s'pose that you would use a second fixturing offset...

But you say that you are moving the part to a different fixture?
Well, no different I guess....

I'm not sure why you would need 2 different programs for this?
I would think that you would use a :

G53 X___ Y0 (bring table up to opperator)

M0 (move part)

M6 T2
M3 S20K
G0 G55 H2 X___ Y___
continue


I've never seen anyone want to run a 2win spindle mill this way, but I guess that if you are running HSSpindle(s) and no tool changer, then I guess I git it, but in this case, you would likely be better suited with a small 16K+ Brother mill for what you want to doo.

???


--------------------------

I am Ox and I approve this here post!

 

[TeachMePlease]

I could be wrong, but this looks like a retrofit of a single spindle machine to use 2x air powered high speed spindles. I wasn't understanding at first how you expected to rough with one tool and finish with another, but I see now. You will used spindle 1 while spindle 2 is off the part, cutting air, and then spindle 2 will finish the part while spindle 1 cuts air. Clever.

 

[solidworks4u]

Ox, and TeachMePlease, thank you for taking interest. This is the few starting lines of G-code after BobCad has generated code for the single spindle parts I have cut in the past.
G90 G80 G40 G20 G17 [this is at the very top]

(Machine Setup - 1-Feature 2 Axis-Pocket)
(FEATURE 2 AXIS)

G00 G90 G54 X-.5142 Y-3.4603 F5. [I need to edit and add the "F5." so it will allow program to run]
G43 H01 Z1. M08
Please take note that no spindle info is provided in the program, because this is manually controlled. There is a parameter in Fanuc to allow the controller to see the spindle is up to speed before the "feed" will start. Think about a broaching operation is how it was described to me, spindle does not rotate, but feed works. I would need to reference my notes for the parameter.

Ox, in your example:
"G53 X___ Y0 (bring table up to opperator)

M0 (move part)

M6 T2
M3 S20K
G0 G55 H2 X___ Y___"

I think I would need to remove the
"M6 T2
M3 S20K"
because this is ATC & spindle control.

After a fresh new program from BobCad, I need to edit the program to add "F5." to the very 1st line of the program, but there are a few other areas that I always look at in the program. I will search G54 (this is the 1st work coordinate) and see if there is a feed at the end of that line in the program, if NO, I will add it.
The post processor is close to providing a near perfect program, I am getting better at editing each program.
As a result of not having everything married together in complete happiness at the post processor, I believe is the reason I will need to start with 2 programs for each part, latter I may find a better workaround.

What I believe is needed to get the 2 spindle program correct, is to keep each "work coordinate" associated with the correct "tool offset" and "tool diameter" for each program. For example, say G54 is the "Ruffing" spindle, it is the larger tool & has a specific "tool offset" required. What I plan to try is a program for ruffing, use the G54 work offset, use the tool offset 01 when setting tool height in spindle, as to "touch off" the surface of the part.

Considering what I have to work with, can I get their form here? I have a picture of the mill, Ox suggest, the small 16K+ Brother mill on the wall & expect that will be as close as I will get to owning one.
Many thanks! All suggestions are welcome.

 

[Matt@RFR]

My opinion is that you will be so much better served by some in-person help. Are there any schools or other machine shops close to you? Maybe you could drop by and ask if anyone is willing to help you with a simple setup in exchange for some cash. I have the feeling that what you need to have done could be sorted in 30 minutes of in-person tutoring, but will take 15 pages of confusion here.

Is there anybody close to Ocean View, DE that could swing by?

 

[MikeBurgess]

What I believe is needed to get the 2 spindle program correct, is to keep each "work coordinate" associated with the correct "tool offset" and "tool diameter" for each program. For example, say G54 is the "Ruffing" spindle, it is the larger tool & has a specific "tool offset" required. What I plan to try is a program for ruffing, use the G54 work offset, use the tool offset 01 when setting tool height in spindle, as to "touch off" the surface of the part.

I think your getting there
Spindle 1 = G54 and Tool 1 offsets
Spindle 2 = G55 and Tool 2 offsets


one thing to really think about is to make sure the non used spindle has clearance in all directions while the other one is cutting.

 

[Ox]

The header on my Fanuc "0M" mill uses G90 G94 G43 G20.

But it is a different machine tool builder, and you could possibly need some others as each MTB has certain defaults set.

On my 0M (I hate the "0" control!) I have learned to not use G54 as on my machine - it defaults to G54 anytime it's not in cycle on a different fixture offset. I don't know why it doesn't default to G53, but mine doesn't. So I like to leave G54 all zeros so that it makes setting others much easier. Yours could be set differently?

Yes, take out the tool change and the spindle start commands, and just feed in inches per minute. (normal)

The biggest thing that I would say is that you want to try out all of your new programs with your Z offset high. Maybe 1" high? Maybe 5" high at first?

Crashing out that spindle will be a bad day!


---------------------

I am Ox and I approve this here post!

 

[solidworks4u]

Matt, thank you!
Mike, thanks! This is correct, my part blank is the highest thing in that zone, over the top of vice jaw by .03" is the bottom of the part, always use CAMotics to proof, the G-code before I go to the mill. I usually "touch off" on top of part blank & know exact thickness of material.
Ox, thanks!! I see what your "header" reads, I may revisit that in my programs. You are not alone with no lost love for the Fanuc OM controller, there are small things that make you wonder, like your G53, if it is MTB or Fanuc thing. I pray the day never comes that Z is too low.
Many, many thanks!

 

[Vancbiker]

...... like your G53, if it is MTB or Fanuc thing. ....

G53 did not become a function on the 0 series controls until the C version. On A or B models it is possible to create a macro program called by G53 that emulates the behavior of "built-in" G53.

 

[MikeBurgess]

I believe in Bobcad you should be able to program it as if your doing a tool change then just go in and edit the Gcode file to add the G54/G55 to each tool change in the program