Problem- Press go-rapid Z into the table!

[Vern Smith]

I fully realize that I can fat finger or confuse myself into pressing the wrong buttons, or the right buttons in the wrong sequence, as good or better then most. However, I have had a situation come up twice that really has me concerned.

A month or so ago I hit feed hold to check something out (not jog away). I then left the program, went to hand jog, and ran the spindle well up so I could get my hands and eyes closer to the situation. When I was ready to go again I paged forward through the program to the tool change that was taken before I hit feed hold (of course the tool was already in the spindle) and hit the go button. I almost crapped my pants because the spindle headed for the basement in G00 fashion. I had it high enough that I was able to catch it before it made it to the table. I tried to duplicate the situation but could not so I chalked it up to some error on my part but I had an uneasy feeling that I had not heard the spindle motor turn on. I've done this same procedure hundreds of times without a problem until this time.

This afternoon I had the same thing happen but I didn't catch it before it exploded a $50.00 carbide EM. It was the same situation, feed hold, hand jog the spindle up out of the way, look at what needed looking at, go to the current tool change and hit go.

This time the proof was in the fixture plate, three indentations from the three flutes, the spindle never started. I guess I need someone to tell me how I managed to start a program at a tool change a few lines before a speed and M03 command, and several lines before any Z commands, with rapid Z results and the spindle motor off?

I'm hoping for a " you dumb a##, everybody knows this happens when you do x then y then z". The thought of this being a random unexplained occurrence to look forward to in the future is a little disquieting.

Maybe the simple answer is to use jog away.

Vern

[gar]

Vern:

You probably do not use the restart function, I don't.

I use a tool change routine that among other things does G90, G5x, speed, start motor, and coolant. And most importance does the tool offset and diameter. I do not include anything to raise the spindle. I have never had a problem starting on an arbitrary call for a tool change of the same tool already in the spindle.

What I have had as a problem is not manually raising the spindle high enough and the X Y following the tool change goes ripping thru the part.

.

[fuzzyracing1967]

I'v done this same thing myself,and I don't have a clue why it does that.The only thing I can tell you is I got in the habbit of just hitting the reset button and then starting from the tool change.

[Geof]

Originally Posted by Vern Smith ...... It was the same situation, feed hold, hand jog the spindle up out of the way, look at what needed looking at, go to the current tool change and hit go....

I am puzzled. Why do you use this procedure instead of Jog Away or simply stopping the program with Reset and then doing a proper Restart with Restart turned on?

[Ken_Shea]

Hi Vern,
Here is some Haas text on "Run-Stop-Jog-Continue


This feature allows the operator to interrupt program execution, jog away from the part to perform a desired task, and then return to the interruption point and resume program execution. Once RSJC is initiated, the operator is able to stop and start the spindle, jog the XYZ axes individually (axes other than X, Y, and Z cannot be jogged), or command a tool release. The following describes the RSJC procedure. (Any Mill Control ver. 11.10 and above)

1) While a program is running, press FEED HOLD. This will stop all motion (after any canned cycle in process has been completed).

2) Press X, Y or Z followed by the HANDLE JOG key. The control will store the current X, Y or Z position. (Axes other than X, Y, and Z cannot be jogged.)

3) At this point, the control will display the message JOG AWAY, and will tick once each second or so. The operator can use the jog handle, remote jog handle, the HANDLE JOG increment buttons (.0001/.1, .001/1., .01/10., .1/100.) or the JOG LOCK buttons to move the tool away from the part.

a) Now you can use the COOLNT key to cycle the coolant, and CW, CCW, STOP to operate the spindle. You can also use the TOOL RELEASE button, and turn Through-Spindle Coolant (TSC) on and off using the AUX CLNT key (note: use of this key requires that the spindle be rotating and the door closed).

b) At this point tools can be swapped out and the associated length and diameter offsets adjusted. However, when the program is continued, the old offsets will still be used for the return position and for any motion commands already in the queue. It is therefore unsafe to swap out tools and adjust offsets when the program is interrupted during a cut.

4) When you’re ready to continue, jog to a position as close as possible to the stored position, or to a point where there will be an unobstructed rapid path back to the stored position.

5) Return to the previous mode by pressing MEM or MDI/DNC. The control will only continue normally if the mode that was in effect at the time of the interruption is re-entered.

6) Press CYCLE START. The control will display the message JOG RETURN and rapid X and Y at 5% to the position where FEED HOLD was pressed; then it will do the same for Z. The rapid rate override keys have no effect during JOG RETURN.

a) Note that the control will not follow the path the operator used to jog away. Instead, it will perform simple moves without regard for obstacles; therefore, a crash is possible.

b) If FEED HOLD is pressed during this motion, the control will go into a feed hold state and display the message JOG RETURN HOLD. Pressing CYCLE START will cause the control to resume the JOG RETURN motion. When the motion is completed, the control will again go into a feed hold state.

[Vern Smith]

Your puzzlement is probably a result of my lack of understanding of the Haas control programming. The only way I have been able to go directly to hand jog is after an M01. If I try to do it after a feed hold it tells me to reset, so I reset. My leaving the feed hold status was always through the reset button because I was not aware of any other way to get there.

Below is my tool change post sequence. It slavishly reproduces itself courtesy of my CAM program. I know this is not a popular way to create G code with our more enlightened members but it usually keeps retreads like me out of serious trouble. I think it includes all the elements Gar has in his.

N5 T8 M06 (AA VERN 1" INSERT 3 FLUTE EM)
N6 G10 L12 G90 P8 R1.
N7 G90 G80 G40 G113
N8 S4200 M03
N9 G43 H8
N10 /M08
N11 G00 X-5.8975 Y-1.6779 Z1.

I agree, "jog away" will I hope circumvent this situation, but why does it happen in the first place? How does the machine control find a way to rapid in Z while ignoring all the commands that started it in motion? The operator, me, must be doing something to enable this situation, other wise Haas would be flooded with complaints.

Vern

[Vern Smith]

Ken,

Your posted information is precisely where I'm going in the future and thanks for saving me the time to find it in the manual. Having never had much success fighting city hall ( with the single exception of getting a one way alley sign removed 30 plus years ago) I will now follow the Haas Commandments and use jog away.

I'm still uneasy about the situation but will let those more proficient deal with it when it happens to them. What are you doing up so late?

Vern

[Ken_Shea]

Originally Posted by Vern Smith Ken, What are you doing up so late? Vern

UH, who are you and what have you done with Vern ?

[Donkey Hotey]

This is going to sound paranoid but the only thing I can add is to use the 5% rapid button.

I always, always, always press that button before restoring motion to the machine in mid-cycle. I watch the cutter and keep one finger on the Start button and another finger on Feed Hold. I don't go back to normal rapids until the cutter is re-engaged and safely cutting.

[Ken_Shea]

Hi Greg,
Good suggestion, better advice.

Ken

[gar]

080329-0744 EST USA

Vern:

I do not see a G5x in your tool change. I believe that newer HAAS controls default to G54 following RESET and some other conditions.

Thus, if in your program prior to this tool change a different G5x from G54 was selected, then you might be working with an incorrect Z reference because the RESET defaults to G54.

Also if you do a G52 on Z someplace in the program you could get an incorrect Z position. How G52 is cleared or used is a function of your mode (HAAS, Fanuc, Yasnac). In HAAS mode it is never changed unless you change it. In Fanuc a number of conditions set all G52 components to 0. In Yasnac I believe it is just another G5x.

Enabling RESTART in HAAS would eliminate these problems because the entire program is rescanned from the beginning. This is not possible in drip feed mode because you can not define the restart point, and it might hours to get to the point also.

.

[Vern Smith]

I appreciate all the helpful suggestions. When I'm proofing a new program or after making any changes to the program or offsets I always go to the 5% or 25% rapids and single block. This situation involved a program that I had been re-running continuously for over three hours.

My year old control defaults to G54, I'm using Fanuc mode and program restart is off. A quick question about program restart, as I understood, when it's turned on you can restart a program anywhere, not just at a tool change (which I used to think was a safe bet). If program restart is on and you do start a program from a tool change, not necessarily the beginning of the program, does the control still go back to the beginning of the program and start over?

Vern