Anyone familiar with the Fadal TRM?

[Tarkus]

The company I just started with has a Fadal TRM with full CNC capabilities. Today I wanted to drill some holes in a bunch of pucks and figured I could use the Fadal. I've never used a Fadal control before and nobody else there knows how to get it to run full CNC programs.

After a few hours, I figured out how to get work height offsets and tool height offsets to work, however, I'm left with a problem.

A. This particular machine doesn't seem to have a true home position. this means you can set machine home from anywhere in range of travel. the only thing that seems to have a home is the tool change position when an M06 is encountered, it will go up to Z home and wait. What I've done is decided on one corner of the table to be zero (and Z top) to be home and backed it way from the limit switches .500 on each axis. Is this a proper thing to do?

B. When the program encounters an offset (G54, G55...), it doesn't just pick up the offset, it also moves at the same time. This presents problems if you have a positive offset since the machine wants to go past the limit of travel. I've temporarily solved this by having it move say (G54 Z-4.) where Z is bound to go lower than the positive offset. I'm sure there must be a way to get it to work properly without moving... (Yes, I even tried G91)

C. The same thing occurs when a tool offset (A negative one) is called (eg. G43 H1). why does it move!?!?!

D. When it ends the program (M02, M30), it wants to go back home PLUS the Z offset (I think) tripping the limit switch

Can somebody give me a very short example of a working program with a tool call?

Here's an example of how my offsets are and an example program

Tool offset 1: Length (-10.356) (distance from Z home to table)
Work offset 1: X(-5.5) Y(-2.) Z(2.109) (Distance from table to top of workpeice)

G55Z-3. (if abs(z) is less than offset then trip limit switch)
T1M6 (brings tool back to home position)
S1000M03
G43H1Z.1 (this works ok but not in MDI even without the Z)
G01Z-.1F1.
G00Z.1
M30 (Goes to Z home PLUS some other value, tripping limit)

What am I doing wrong?

Any help is appreciated!

[little bubba]

I'm not familiar with the TRM, but it sounds like the machine is in Format 1, which is basically useless as far as I'm concerned. Its susposed to make programming easier and all it does is make it more aggravating. Switch it over to Format 2, more fanuc based and you shouldn't have a problem.

[nervis1]

The manuals for that machine are at Fadal's website.

[Admirp]

Here's an example of a program, in format 2 however


O0001 ( PROGRAM - 6964T4 )
N100 G90 ( DATE - 27-02-06 TIME - 12:41 )
N102 G20
N104 G0 G17 G40 G80 G90 G94 G98
N106 G0 G28 G91 Z0.
N108 G0 G28 X0. Y0.
N110 ( MIDDLE FLANGE PROFILE CUT ROUGH AND FINISH )
N112 M63
N114 M61
N116 T4 M6 ( 1.25 FLAT ENDMILL T4 D4 H4 DIA.=1.25 )
N118 G0 E1 G90 X-16.7802 Y-.6232 A-0. B90. S1200 M3
N120 M62
N122 M60
N124 G43 H4 Z9.1142 M8
N126 Z7.2142
N128 G1 Z6.9142 F15.
N158 G41 D4 X-16.0852
N160 G3 X-15.4602 Y.0018 J.625
N162 G2 X-9.6827 I2.8888
N164 X-15.4602 I-2.8888
N166 G3 X-16.0852 Y.6268 I-.625
N168 G1 G40 X-16.7102
N170 Z7.0142
N172 G0 Z8.9142
N174 M9
N176 M5
N178 G0 G28 G91 Z0.
N180 G0 G28 X0. Y0.
N182 G28
N184 M30


I'm kinda busy now, so look this over and i'll come back later and add a few things.

[Admirp]

D You have to send it home at the end of the program as in line N178 otherwise it will do what you described. Other option would be to cancel out your g55 callout before the end of the program (if you decide to stay in format 1)

A Fadals have what's called a Cold Start position. You use that as your reference point in a way, after machine has been powered down. Your home can be basically anywhere. I keep my home pos. in x and z same as cold start, and in y with table all the way towards the machine door. That way when at the end of the program you send it to x and y home, you don't have to jog the table around to have your part within easy reach.


I'll be back for some more

[DareBee]

I use my CS as home position as well, in my CAM post processer i have an line added automatically at the end of each progrm to move my Y up to the door, even though this is technically not home.
This is an a 4020 not a TR

[daking]

Tarkus,

Your program looks more complicated than needed. If you wanted to drill a series of holes in a part a sample program in format 1 might look like this:

T1M6
G90G0X1.Y1.(FIRST HOLE POSITION)
S3000M3M8
H1G0Z0(CALL TOOL LENGTH OFFSET 1 AND MOVE TO Z 0
G98G81X1.Y1.Z-1.R0F10.(DRILL AND RETURN TO PREVIOUS Z
X2.
X3.
X4.
G80
M5M9
G49G0Z0(CANCEL OFFSET 1 AND RETURN TO Z 0
G90G0X0Y6.M0(PARK AND LOAD
M2 or M99P1


You don't need to use G43 unless you have some reason to want to.(preset tooling maybe) Just set your clearance height as your offset(H1).
In format 1 M30 is "end of all sub-routines" so use M2 or M99Pxx to return to the start. If you dont have a specific reason for a fixture offset, dont use one . Just set X Y zero where you need to and go. I'm sure some will disagree with this but I've been doing it for ten years. Its simple and it works.

Dave

[Tarkus]

Thanks for the info guys...

Out of curiosity? how do you set your work offsets and tool offsets?

Myself, I set the work offset Z as a distance from the table (or touch pad) to the part, so a positive value (eg. 2 .01)
Then for the tools I set it as a distance from cold start Z to the table (or touch pad) and therefore it is a negative value. (eg -19.2000)

Thus the tool is negative and the part is positive on the Z. The only problem however is that in format 1 I have to call both the E and the H at the same time, making for weird rapid moves.

How do you guys do your offsets?

[little bubba]

To make it easier on yourself, I would take Format 1 and stick it in the chip pan. I don't even know why Fadal has a Format 1 and a usable format.

As for setting tools, if your using a tool length probe, then your doing it the right way and letting Format 1 throw a wrench in the works. I usually set the tools right off of the part, with a fixture offset of Z 0, but then again, its not that often that I'll use the same tools on more than one fixture, also the tools in the carousel are seldom the same, so setting off of the table isn't really an advantage for me. If I was continually using the same tools, or using them on more than fixture, I would set them off of the table.

I guess I could always have my 1/2" rougher in pocket 11, but I don't have the time to wait for the tool changer to get all the way around to pocket 11.

[Admirp]

I prefer to do the offsets the same way as you tarkus. We all use it as a kind of a standard just for the fact that i might not be there one day, and somebody else will need to change tool on my machine. Also every once in a while i will use quite a few tools from one program in the next one on that machine. It's also good to know that all the tools in the turret are set right and from the same place, just in case.


BTW, i wasn't aware that a programming on a TRM would be any different then on a say 4020.

[daking]

I almost always leave z zero at the tool change position and set the tool off the part or some other reference. I occasionally use fixture offsets but not often. Usually stay with E0 unless running multiple parts at one time. I usually try to keep the work to the z minus side. We don't have any Fanuc type machines so we just use Format 1.

I've seen people bash Format 1 in this thread and others. I've never seen an actual example of why Format 1 is so bad or why Format 2 is better. What can Format 2 do (other than run Fanuc type programs ) that Format 1 can't? I don't use Format 2 because I don't need to but I'd really like to see what the difference is. We've been using Format 1 since we got our first Fadal in 1990. We have'nt found anything we could'nt do because of it.

[TR MFG]

While I've never run a TRM this info should apply. I always used format 2, only because the machine I trained on was set up that way the shop had some machines with Fanuc's. Why use format 1 verse 2?
I always set my tool length on the top of the part or some other reference, giving a negative tool length from the cold start position. I always would use "E" fixtures, leaving the Z value zero. I tike to use fixture offsets because I would frequently run more than one part, or while I was in the middle of a run I would need to do something else.
I also changed the home position so the table would come to the front at the M30 command. I believe the command to set the home position was to cold start, jog to the new home then do HOSET. Then next time you power up it will prompt you to return to the last home position. I don't currently have a Fadal in the shop so some of this info may be a bit rusty.