Expensive lesson

[RustedOut]

Man, and I knew better too. Decided to add a ream operation at the end of a new program, really not to run the ream operation, but to have the x and y locations and the final depth of the reamer right there in the program to keep from needing to write them down. Got it done and loaded the program and the mill head came rapid down into the top of my vise. Forgot the mandatory M03 and spindle speed prior to a G86 (my mill is manual spindle operation so never use them).

The spindle was only about an inch and a half above the vise at the time and came down so fast I couldn't react quick enough. One other thing I forgot to do was hit the reset button before I loaded the new program. You know, you think you got it all figured out after 30 or 40 programs. The first time I used a G86, the head went the other way, but had a ways to go to the top so I got it stopped. I think I'll get into two habits here, add the spindle on and speed values and a spindle stop at the end of each operation on every program, and hit the reset button before loading the new programs.

Now I have to replace the bent 3/4" ballscrew. Bent it just above where the nut was at the time, about 14 to 17 inches down from the top of the column. That is exactly where the majority of my programs have been running lately. The bend causes the head to stutter, even at low feed rates. It travels good a few inches above the bend.

Hope this keeps someone else from the same fate. At least it was the shortest ballscrew and I don't think it messed up the nut. Now I really need to finish my thread die holder for my lathe.

Bob

[Shev]

Bummer...I guess if I bent a screw I'd want it to be the short one...post pics of the repair processs...

[WayneHill]

Good lessons come from bad experience.

[Cruiser]

That ball screw should not have bent ! I have had hits too, many of them, hard and destructive. The ball screw shouldn't bend. find out what else is wrong and then replace what you have to. I'd start by looking at the lug fitment to the Z saddle. If it has a lot of play it may need to be bushed to take up all of the slop. If it is getting cocked down from the thrust then you will have the problem again till it is fixed correctly.

[RustedOut]

That ball screw should not have bent ! I have had hits too, many of them, hard and destructive. The ball screw shouldn't bend. find out what else is wrong and then replace what you have to. I'd start by looking at the lug fitment to the Z saddle. If it has a lot of play it may need to be bushed to take up all of the slop. If it is getting cocked down from the thrust then you will have the problem again till it is fixed correctly.

Thanks for the advise Don. I had intended to take the whole Z pieces off and take a look. I've wanted to replace the cap screw at that attachment. This may have stretched it even more. I do have the larger 1125 oz in motor on that axis and am thinking that's what did it in. It runs in a four to one ratio, so there is a lot of force there.

Right now am waiting on a price quote from Rockford for a replacement. Need to make an outboard spindle spider and tail stock die holder for my lathe to be able to turn and thread the new screw. I can work on those till the replacement comes.

Bob

[mactec54]

RustedOut

Post the program that you crashed with, there may be other code in your program that caused your problem, a G86 is not going to cause you a crash, it's what was before the G86 is were the problem is

[Dave.Kellogg]

With larger motors, would it make sense to design-in a shear pin in the axis drive train to guard against such crashes? This would function as a mechanical "fuse", and serve as a line of protection.

[RustedOut]

It has a shear pin right at the motor shaft to the pulley adapter. It's a 3/32 hollow pin. Didn't shear this time but did one other time when I set Z0 to the wrong value. It hit harder this time than the time before. All my motors have them.

I'm thinking a better solution is the err/res post coming out of the Gecko's. Possibly add in a momentary switch to reset them on startup, then if the drives fault for any reason, they won't automatically reset. The way it's wired right now is with a jumper from err/res pin to enc+ pin. Always been of the mind set that it would be nice to have it setup that way, but I'd like to have one reset button for all the drives, with individual led's for indicating which drive faulted. Haven't got that entirely figured out yet. I'd want them right on the enclosure door. Not really an electronics type although I've done most of it so far. So, if what I'm thinking if that part of the Gecko's is true, the drive faults once and can't be reset so it should minimize any damage. Anyone done theirs that way?

Here's the program, but now with an M3 and S190 right ahead of the G86. Without that somewhere in the program, soon as the program loads, the Z takes off at rapid speed. Haven't figured out exactly what tells it which direction to go either. Probably the "Z-1.9287" in this case. I've just never really used a G86 much before. Loads fine as is and I ran another just like it drilling, milling and reaming from the other side before I reset the block and loaded this program. It's Z0 was on the bottom of the stock though and had a +Z value for the bottom of the reamer. And when I loaded it I had hit the reset button before hand. Still had to edit the program to add the M3 and spindle speed before it would run.

You can see I do use the tool height and load tool statements even though I don't currently use preset height tools. I plan to get there soon though. And a funny thing, I used to add the M3 and S values to all my programs as instructions to myself as PP instructions in the programs during creation.

%
O1000
N1 G49 G54 G20 G80 G40 G90 G94 G17 G98
( Cliff Lott's Saw Brackets )
N2 (C01 drills and reams through hole to 3/4)
N3 (Uses spot drill, .2188, 1/2 & 5/8 drills, 1/2 x 2" loc EM and 3/4" reamer)
N4 (Set Z0 at top of stock, Y0 opposite movable jaw, X0 on left corner)
( T1 Spot Drill D 0.591 )
N5 T1 M6
N6 G0 X.7 Y1.7455 S1600 M3
N7 G43 Z1.5 H1
N8 G1 Z.5 F11.8
N9 Z.25 F9.6
N10 G81 X.7 Y1.7455 Z-.04 R.25 F9.6
N11 G80
N12 G1 Z1.25 F39.4
( T2 Drill D .2188 )
N13 T2 M6
N14 G43 Z1.25 H2
N15 G1 Z.25 F40.
N16 G83 X.7 Y1.7455 Z-2.3157 R.25 Q.075 F9.6
N17 G80
N18 G0 Z1.25
( T3 1/2 Drill )
N19 T3 M6
N20 G43 Z1.25 H3
N21 G1 Z.25 F40.
N22 G83 X.7 Y1.7455 Z-2.1943 R.25 Q.12 F5.5
N23 G80
N24 G0 Z1.25
( T4 5/8 Drill )
N25 T4 M6
N26 G43 Z1.25 H4
N27 G1 Z.25 F40.
N28 G83 X.7 Y1.7455 Z-2.2304 R.25 Q.15 F5.5
N29 G80
N30 G0 Z1.25
( T5 End Mill 3002 )
N31 T5 M6
N32 X.6667 Y1.7022
N33 G43 Z.53 H5
N34 G1 Z-1.97 F40.
N35 G3 X.7345 Y1.6823 I.0439 J.024 F14.4
N36 X.7345 Y1.6823 I-.0345 J.0632
N37 X.7544 Y1.7502 I-.0239 J.0439
N38 G0 X.6715 Y1.6935
N39 G3 X.7393 Y1.6735 I.0438 J.0239
N40 X.7393 Y1.6735 I-.0393 J.072
N41 X.7592 Y1.7414 I-.024 J.0439
N42 G0 X.6763 Y1.6847
N43 G3 X.7441 Y1.6648 I.0438 J.0239
N44 X.7441 Y1.6648 I-.0441 J.0807
N45 X.764 Y1.7326 I-.024 J.0438
N46 G0 X.6811 Y1.6759
N47 G3 X.7489 Y1.656 I.0438 J.024
N48 X.7489 Y1.656 I-.0489 J.0895
N49 X.7688 Y1.7238 I-.024 J.0439
N50 G0 X.6859 Y1.6671
N51 G3 X.7537 Y1.6472 I.0438 J.024
N52 X.7537 Y1.6472 I-.0537 J.0983
N53 G1 X.7561 Y1.6428
N54 G3 X.7561 Y1.6428 I-.0561 J.1027
N55 X.7561 Y1.6428 I-.0561 J.1027
N56 X.776 Y1.7107 I-.024 J.0439
N57 G0 Z.53
( T6 Reamer D 0.75 )
N58 T6 M6
N59 M3 S190
N60 X.7 Y1.7455
N61 G43 Z.25 H6
N62 G86 X.7 Y1.7455 Z-1.9287 R.25 F1.5
N63 G80
N64 G0 Z2.
N65 X0. Y0.
N66 M30
%

[mactec54]

RustedOut

Your program is almost ok, the depth should be -.750 & not -1.9287 the only thing you should check is the T6 H6 to see if the reamer was set to the top of your part

Also a G86 is normally for Face Boring cycle, but this would not of made it crash, most likely was the tool setting

Are you using a tool changer

For a reamer try this

T6M6
G54
S190M3
G90G0X.7Y1.7455
G43Z.25H6
G85G98X.7Y1.7457Z-.75R.25F1.5
G80G0Z2.
M5
G0X0.Y0.
M30

[RustedOut]

RustedOut

Your program is almost ok, the depth should be -.750 & not -1.9287 the only thing you should check is the T6 H6 to see if the reamer was set to the top of your part

How do you figure that? It needed to go just above where my 1/2' end mill bottomed out at around -1.97. The part I'm cutting is 1.75" wide and the hole goes all the way through, so the 1.9287 value got me there.

Z0.0 would have been set at the top of the stock if I hadn't crashed it prior to getting to that point. And I never got to the point of setting any tools. It crashed on loading the program, no cycle start.

Also a G86 is normally for Face Boring cycle, but this would not of made it crash, most likely was the tool setting

Are you using a tool changer

For a reamer try this

T6M6
G54
S190M3
G90G0X.7Y1.7455
G43Z.25H6
G85G98X.7Y1.7457Z-.75R.25F1.5
G80G0Z2.
M5
G0X0.Y0.
M30

The G86 was the G code I got after posting my program and I choose a ream operation in my CAD package. I'm pretty sure that it was a power down, spindle off, manual out, but I'd have to check to be sure. Like I said, I don't normally do that, but it seemed a good way to get it written down for me. I wasn't brave enough to let it run through the operation. I would have had to run it in the air before I could get to that point and didn't want to waste the time yesterday.

I'd have thought a G87 (manual out) would have been more appropriate, but couldn't correlate my CAD choices to that particular G code. Something else to put on my to do list. Puzzles me where the M5 should be in that line. Think I'll play with that some more while I'm waiting to fix my mill.

And no, no tool changer. The majority of my programming has been with high speed routers, newer 3 axis mills and older 5 axis mills with either tool length comps or tool changers and tool setters, so that is just a habit I've carried into my home programming. I'll never have a tool changer though, but will have a method to preset the tool length soon.

I'm kind of thinking that taking off like that on loading the program may be a small problem in Mach3 although I've seen some weird things caused by missing decimals or H values on Fanuc controllers in the past. At least Mach give you messages of errors, it's just this one came with rapid motion as well with no cycle start.

Bob

[mactec54]

RustedOut

The -.750 I though that was how deep you were going,With Mach taking off like that we have never seen it do that, & I don't know how it can

The G85 is feed in feed out, which is best for reaming

You also have to have a G90 or a G91 to tell the control what it has to do & how it's going to move, for the M5 if you have a M3 to turn the spindle on you want to have a M5 to turn it off You can put it anywere you want once it has finished cutting

Between each program if you want to do them like you have, you will need to have a M0 or a M1, M0 for program stop M1 for Optional Program Stop You need this if you don't have a tool change

Go through through the Mach set up manual, & try to see what went wrong, it was not the program that made it crash/ start by its self

http://www.machsupport.com/docs/Mach3Mill_1.84.pdf

[RustedOut]

RustedOut

The -.750 I though that was how deep you were going,With Mach taking off like that we have never seen it do that, & I don't know how it can

Yea, surprised me a whole lot, but that happened on merely loading the program. First time I had been setting my part machining axis by jogging around to find the edge of the stock. So the reset was enabled. Then loaded the program and the Z took off all on it's own. Fortunately it was going up and I was able to hit the emergency stop button and prevent it from doing any thing.

This was the second time and I had forgotten to add in the M3 and rpm, or hit the reset before loading it up. And this time it went down right into my vise.

The G85 is feed in feed out, which is best for reaming

I like to feed down and stop the spindle then retract the reamer and sometime like doing a boring head that way as well. Maybe a G88 is the better choice for that.

You also have to have a G90 or a G91 to tell the control what it has to do & how it's going to move, for the M5 if you have a M3 to turn the spindle on you want to have a M5 to turn it off You can put it anywere you want once it has finished cutting

I understand the M5's and M3's well enough, but I guess I'm not understanding what a G90 or G91 has to do with the G86. I'm already right above the area to be reamed, just need to go down to the specified Z level and retract or not. If I'm in incremental already, that's what my Z move will be, at least in my thick head.

Between each program if you want to do them like you have, you will need to have a M0 or a M1, M0 for program stop M1 for Optional Program Stop You need this if you don't have a tool change

Go through through the Mach set up manual, & try to see what went wrong, it was not the program that made it crash/ start by its self

http://www.machsupport.com/docs/Mach3Mill_1.84.pdf

Are you saying each of my operations is a separate program. I don't treat them like that. My programs get pretty lengthy as I run a number of cutters to get the part finished to a specific level in each machine position. This part is actually two parts exactly alike made from a single stock. They are tabbed clear up until the last cutter is withdrawn, then separated. There are 4 positions and 4 different programs each having multiple cutters.

The parts I just finished had just over 9000 operations and 8 different cutters all in one position making three parts at one time. No machine stops anywhere, just load tool statements. Z was set for each tool while in a tool change operation. Took over 4 hours run time, but it worked fine.

Thanks for the info. I'm still learning my CAD and how it relates to Mach3, but am getting there. Hope all this makes some sense.

Bob