[triumph406]

Hi to all the Fadal experts!

I have a new to me '91 4020. I've machined a few parts OK on it, but am stumped at times why it does the unexpected. I have run a Makino with a Fanuc 0m for years, so not a newbie.

The machine is configured for Format 2 in G90 (absolute mode)

The part in the vice has the upper far left hand corner set as X0Y0Z0. I set the XYZ in MDI using G92, with appropriate X or Y value accounting for edge finder diameter, and set Z with a block under the tool. I've also set X,Y,Z using SETX/SETY/SETZ, still the same behaviour.

In the offset table I offset all the tools +3" in Z to run high above the part.

The first tool is T10 (1/2 EM)

When running programs I run using slide hold for the 1st pass, when I ran it for the 1st time I could see the -Z distance to go was to great, so I stopped the program, jogged it in -X and -Y away from the part and vise, and started the program again. The result is the video.

https://www.youtube.com/watch?v=r3nf...ature=youtu.be

The program starts by going up to the toolchange position, plunges down below the part before the spindle starts, then rapids up to where it starts it's 1st G1 move in +Y.

The program start is below. So what am I missing?? I've tried Format 1 and 2, I've tried both Fanuc and Fadal posts nothing makes a difference. The E1 values are X0,Y0,Z0. Is it picking up an offset from somewhere that I can cancel at the begining of the program? I don't understand why it plunges down before the spindle starts. I ran a Fadal in the mid 90's and can't remember any of these issues. There's probably plenty of other mistakes in the program.

Thanks in advance for any help you can provide!!

Is the 'whine' from the spindle common, it sounds like a VFD issue, it goes away at higher speeds

Dave

%
O0003
G17 G40 G80 G90
T10 M6
M3 S3000
G0 X-0.25 Y-2. G43 Z0.5 H10
M7
G0 Z-0.4
G1 Z-0.6 F47.7
Y0.5 F60.0
G0 Z0.5
Y-2.
Z-0.4
G1 Z-0.6 F47.7
Y0.5 F60.0
G0 Z0.5
X26.25
Z-0.4
G1 Z-0.6 F47.7
Y-2. F60.0
G0 Z0.5
Y0.5
Z-0.4
G1 Z-0.6 F47.7
Y-2. F60.0
G0 Z0.5
M9
T1 M6
M3 S2000
G0 X0.75 Y-0.75
G43 Z1. H1
M7
G81 X0.75 Y-0.75 Z-0.18 R0.1 F2.2
X7.
X8.5
X10.
X11.5
X13.
X14.5
X16.
X17.5
X19.
X25.25
G80
M9
T6 M6
M3 S2000
G0 X0.75 Y-0.75
G43 Z1. H6
M7
G83 X0.75 Y-0.75 Z-0.7 Q0.2000 R0.1 F2.2
X25.25
G80
M9
T2 M6
M3 S3000
G0 X7. Y-0.75
G43 Z1. H2
M7
G83 X7. Y-0.75 Z-0.7 Q0.1500 R0.1 F4.0
X8.5
X10.
X11.5
X13.
X14.5
X16.
X17.5
X19.
G80
M9
T21 M6
M3 S300
G0 X7. Y-0.75
G43 Z1.5 H21
M7
G84 X7. Y-0.75 Z-0.6 R1. F12.5
X8.5
X10.
X11.5
X13.
X14.5
X16.
X17.5
X19.
G80
M9
G90
M30
%

[triumph406]

This morning the machine did the same thing again, plunged below the starting Z before the spindle would start.

So instead of starting with tool 10, I put Tool 9 in the spindle, it did a toolchanger to Tool 10 and then the spindle started normally as it was rap using down to the part. Not sure why that would work any differently but it did.

I ran the program 3" high, the last move of the tap holder was to plunge down towards the part , is this because of the G80 at the end of the program?

[triumph406]

I added a G0 Z10. at the end of the program, the tap still tried to rapid down in Z.

T21 M6
M3 S300
G0 X7. Y-0.75
G43 Z1.5 H21
M7
G84 X7. Y-0.75 Z-0.6 R1. F12.5
X8.5
X10.
X11.5
X13.
X14.5
X16.
X17.5
X19.
G0 Z10.
G80
M9
G90
M30
%

So what fundemantal Fadal knwoledge am I missing?. I've had more issues trying to program the Fadal on a few parts, over a few days than with my Makino over 15 years.

[mactec54]

I added a G0 Z10. at the end of the program, the tap still tried to rapid down in Z.

T21 M6
M3 S300
G0 X7. Y-0.75
G43 Z1.5 H21
M7
G84 X7. Y-0.75 Z-0.6 R1. F12.5
X8.5
X10.
X11.5
X13.
X14.5
X16.
X17.5
X19.
G0 Z10.
G80
M9
G90
M30
%

So what fundemantal Fadal knwoledge am I missing?. I've had more issues trying to program the Fadal on a few parts, over a few days than with my Makino over 15 years.

You have the G80 in the wrong place, you need it before the Z move, in your first program, that is a crash waiting to happen, never have a rapid move X Y & Z in the same line Z should always in this case,should be separate, as you have done in this last program

[triumph406]

You have the G80 in the wrong place, you need it before the Z move, in your first program, that is a crash waiting to happen, never have a rapid move X Y & Z in the same line Z should always in this case,should be separate, as you have done in this last program

mactec,

In the 1st program I have the G80 after the last X move, the z-axis will plunge after the tapping retract
X16.
X17.5
X19.
G80
M9
G90
M30
%

In the 2nd program, if that was run on the Makino, the z-axis would go to Z10 before the spindle stopping, but with the 4020 it still wants to plunge down in Z. ( I forgot to check what the distance to go was to see if I could figure out what Z value it was trying to go too)
X16.
X17.5
X19.
G0 Z10.
G80
M9
G90
M30
%

What does it achieve to put the G80 infront of the G0 Z10 on a Fadal?, I'll try that in the morning to find out I guess.

I hear you on the G0 xyz moves on the same line. If the parts above the top portion of the vise, and I know the Z is above the part top Z then I don't worry about a crash, on the other hand, if the part is held down with clamps, then the first G0 move would be XY, and the next line would be the Z move.

[mactec54]

triumph406

If you have been programing this long, you should know what each piece of code does, and how it is used, the G80 cancels the Canned cycle which has to happen before the next movement

Some controls this does not matter,and the G80 is not needed in the program, but if you are using different machines/controls then it's best to just leave it in the programs in the right place, and it will suit all machines

It does not matter what machine you are programming, your G-Code format needs to be changed to have reliable machine running

[triumph406]

triumph406

Some controls this does not matter,and the G80 is not needed in the program, but if you are using different machines/controls then it's best to just leave it in the programs in the right place, and it will suit all machines

Correct the Fanuc 0m does not require a G80, a G0 after the last X move will send it where I want, The Fadal seems to be a different story. Putting the G80 before the G0Z10. did the trick thank you.

[rodney247]

Dave,

The problem why your Z is going so far down is because you used SETZ setting your Z zero at spindle nose to top of part do not do that ( so right after the tool change the machine is going to the SETZ position) Re do it and SETZ at the ColdStart (machine Home) Z axis CS. Then Set all your tools from this point with your Z zero Set at coldstart. So when you type in the control and type HO at the enter next command prompt your Z should go to the CS mark (which is ToolChange position) Use the UT command to set all your tools.

When your running only one Fixture offset Normally your Z in the Fixture offset should be Zero. If running 2 fixtures offsets say lets say 2 vises you would have a different X and Y value (new corner of part) and you would use the Z offset in that fixture to compensate the difference of the 2nd Vice. This will solve your problem.

Also your Orientation factor in the SETP is too high thats one reason the machine is having trouble orientating. go to the SETP and drop the number down a couple of numbers hit manual and re CS the machine and check the orientation speed M19 in MDI.

What happened is which is very common from people that are use to FANUC machines and then try to run a FADAL is that they think FORMAT 2 turns the machine into a machine that is Run and Setup like a Fanuc. Format 2 is Fanuc compatible. It runs Fanuc Programs, but it is still a Fadal.

Next time you run a Fanuc see if they give you a FADAL compatiblity option................ lol ,,,, that was just a little humur joke they don't.

If what i said doesn't make sense give me info a i can talk you thru it. Have a great day.

[triumph406]

Dave,
The problem why your Z is going so far down is because you used SETZ setting your Z zero at spindle nose to top of part do not do that ( so right after the tool change the machine is going to the SETZ position) Re do it and SETZ at the ColdStart (machine Home) Z axis CS. Then Set all your tools from this point with your Z zero Set at coldstart. So when you type in the control and type HO at the enter next command prompt your Z should go to the CS mark (which is ToolChange position) Use the UT command to set all your tools.

I would assume then that all the tool offsets would be negative values (as set in the offset table the previous owner had setup)
In that case I assume I should be in G91 mode? So the the Z I set the top of the part too will be in relationship to SETZ?
Currently I’m using G90 mode, and all my tool offsets are positive. I set the tool height using G92Z(insert value)

When your running only one Fixture offset Normally your Z in the Fixture offset should be Zero. If running 2 fixtures offsets say lets say 2 vises you would have a different X and Y value (new corner of part) and you would use the Z offset in that fixture to compensate the difference of the 2nd Vice. This will solve your problem. .

Might be running 2 vises next week, bet that’s going to be fun!

Say I write a program to face of a piece of stock mounted in a vise, and for whatever reason it doesn;'t cleanup, Do you edit the X value in the Fixture offset to then take off more material?

Also your Orientation factor in the SETP is too high thats one reason the machine is having trouble orientating. go to the SETP and drop the number down a couple of numbers hit manual and re CS the machine and check the orientation speed M19 in MDI. .

Most of the time it finds the orientation in a turn, but I will reduce the value as you suggest. I did wonder why sometimes it had trouble orientating.

What happened is which is very common from people that are use to FANUC machines and then try to run a FADAL is that they think FORMAT 2 turns the machine into a machine that is Run and Setup like a Fanuc. Format 2 is Fanuc compatible. It runs Fanuc Programs, but it is still a Fadal. .

I think my initial thought was that format 2 would make the machine more Fanuc than Fadal, any illusions I’ve had that I would up and running and productive in a few hours are long gone. I thought at least the programs would be compatible between Fanuc 0M and Fadal, which is largely true, with a few exceptions.

Next time you run a Fanuc see if they give you a FADAL compatiblity option................ lol ,,,, that was just a little humur joke they don't. .

If I fired up the Makino, and it asked If I wanted it to be Fadal format for a day, I’d jump off the building!!

If what i said doesn't make sense give me info a i can talk you thru it. Have a great day.

Thanks for the offer, I may take you up on it!

[rodney247]

Dave make your life easy and set your tools using the UT command

Your program will be run in G90

forget the G92 thing (your mind is in total Fanuc mode) lol SETX SETY SETZ is a fadal thing it sets the machine coordinates to 0,0,0

You can use the UT command to pick up the fixture offset automatically too. or pick up JUST your X and Y location and enter that into the DF. X(value) Y(value) Z (zero) your next fixture 2 will be X(value) Y(value) Z(.02) <--difference in the height of vice possibility

So step 1 setup tool lengths using the UT command it is conversational just fill it the blanks which tools your setting and if your using a 1.00 block to pick up the tools, and basically just follow the prompts on the screen.

Step 2 pick up the part corner using UT conversational although might be easier just to go to the DF command and enter the values for the Fixture you want.

Step 3 Load your program and hit auto.... lol

- - - Updated - - -

or if your not busy pm me your number and i will talk you thru it

[triumph406]

or if your not busy pm me your number and i will talk you thru it

PM sent.