Hass CNC MILL TM 1P PARAMETER #23

We are having issues with our Hass CNC mill , Our program was written on ESPRIT and it runs okay , except that it will no let use cutter compensantion during an arc milling op. , we contacted HASS TECH SUPPORT they also tested our program and did not find any issues with the program as it is ,the control prompts a 104 alarm , indicates that parameter #23 Y MAX ERROR is involved , the actual value is 16384 , question does any one owns or works with a Mill of this model that perphaps can help me to see if the parameter set on my machine is correct ? appreciate any help .

I am not sure exactly what this parameter is for, but on my TM2P, it is set to 131072.

G00 Proto said:

I am not sure exactly what this parameter is for, but on my TM2P, it is set to 131072.

Click to expand...

Thanks for replying to my post , I would like to know what some else has on a TM 1P ,by the way the reason I am on this search is because I am having issues with the machine not allowing me to use the tool wear to compensate on G02/G03 , I got a program wrotte with Esprit , double check already with the Esprit guys and programming is good but for some reason the machine will not take any values on tool wear during arc milling , Iam properly using G41 / G42 and the alarm 104 or I get a I j or k not allowed with G02/G03 have you ever had any issues like that , regards.

2007 Haas TM-1P here. I haven't used tool wear comp, only tool radius comp on this machine.

FWIW, my machine has the following: on page Y PARAM A, Y MAX ERROR (param. #23) = 16384


HTH,
M

mountie said:

2007 Haas TM-1P here. I haven't used tool wear comp, only tool radius comp on this machine.

FWIW, my machine has the following: on page Y PARAM A, Y MAX ERROR (param. #23) = 16384


HTH,
M

Click to expand...

thanks for the info , I have used Tool wear for years on this machine , the last program is an arc milling of a part mounted on the 4th axis , the radius is 3.65 ´´ , it does it as long as I don´t use any values on the tool wear , I generated again the arc with mini lines and executed on G01 and it will let me used Tool Wear as I need but there are other features a DOME that needs to be cut as well , there I have to used G02/G03 moves and that is where things get complicated it will not let me used not even .001´´ tool wear ,been doing this a while a never seen a machine act like that be it a swiss lathe , CNC LATHE or CNC MILL as long as G41/G42 is programmed it should compensate, regards.

fer-va said:

I generated again the arc with mini lines and executed on G01 and it will let me used Tool Wear as I need but there are other features a DOME that needs to be cut as well , there I have to used G02/G03 moves

Click to expand...

emphasis mine

From your description it seems you're cutting a 3D path. Once you use G02/G03 (for either smoothing or to lessen the number of small moves made), I'm guessing the control doesn't know what to do in 3D. I'll bet tool wear works fine in G17 (XY plane), but the control may barf in G18 or G19. Again, I'm just guessing here, so take that as you will.

From the sounds of it I doubt a parameter change to the machine will fix the problem.

1. Find what moves it doesn't like and fix them. You say you are using lots of little moves. Some lines or arc moves some are probably smaller than your wear amount. Does a smaller tool give larger arc moves that can then be comped?

Or

2. Just use your cutter dia in cam as your wear adjustment and repost the code and move on with life.

Just some general things. If you can post a snippet of code where the alarm is and a picture of the alarm, or exactly what the machine alarm says, someone can probably tell exactly what the problem is. But it is a pretty normal problem where arc moves are not much at all. Or short line moves sometimes.

Thanks to everyone , I mentioned that I ended up creating the arc on short lines simply because when I import the solid from solid works to Esprit on IGS. format it will always explode arcs into small segments or most of the time I should say , so is easy to create a chain feature that Esprit will put out a whole bunch of small moves on G01 ,that is the easy part , to get an arc created on G02 or G03 I had to redraw it , once it is imported to ESPRIT, the thing is that the geometry is fine as well as the I ,J coordinates generated for the center of the arc ,I could use option #2 but I have at least a 1000 parts to make on stainless 304 so I must be able to use Tool wear to keep al the features on tolerance , the quality sampling is done on AQL basis so is pretty strict , thanks a lot to everyone that has posted on the matter .

I occasionally have that problem. I think it is when the lead in arc is insufficient to engage cutter comp. I usually run into it when I am circle milling the inside of a bore, and the bore is very close to the diameter of the cutter.

I will say that the very first thing I do when I am programming is to get rid of as many segmented arcs and lines as possible (ie splines). I want the machine to process as few lines of code as possible. Cam systems break up splines into very small line or arc segments that cause machines to slow down, stutter and leave witness lines on the parts. Unfortunately, coming from the solid, any line that would be an arc, but transitions in the Z is interpreted as a spline... 1000 lines of code that could be replaced by one arc move. (and no, programing off of the solid does not fix this)

If you are trying to program off of one of these spline segments, the line or arc may not be long enough for the Haas brain to process. At the end of the day, the Haas control is not very sophisticated and doesn't process spline type geometry very well. Do a little house cleaning on your 2D geometry by replacing the splines with 3 point arcs and your life will be much easier.

Thanks a lot for your notes , it seems indeed that it is a Hass control limitations issue , actually the line of code is pretty lean as it is a yet it will stall right at the intersection of the arcs , I had Hass people to look at my program and Esprit tech support as well an yet can get nobody to find the cause of this matter my lines of code where it stalls :
N89 G01 Z.556 F20.
N90 G1 G41 D4 Y1.5212
N91 G2 X-4.5015 Y1.6565 I.1449 J-.0051
N92 X-4.4667 Y1.6604 I.0312 J-.121
N93 G3 X-3.3186 Y1.8177 I.102 J3.5235 RIGHT at this line it will give an alarm I ,J or K not allowed on G02/G03 ,it will execute it as long as I dont have any values on my TOOL WEAR page , thanks , regards

The controller reads ahead also, the offending line may be past where the program actually stopped execution. Single block thru the program may stop the program on the line with the actual problem. So, you, or us, need to see more of the program.

Does it alarm with a negative value in the wear comp? Sometimes on tight spots I will program my tool .001 to .002 oversize (.0955 for a 3/32 em for example) then zero comp will leave stock and I can negative comp to size.

fer-va said:

Thanks a lot for your notes , it seems indeed that it is a Hass control limitations issue , actually the line of code is pretty lean as it is a yet it will stall right at the intersection of the arcs , I had Hass people to look at my program and Esprit tech support as well an yet can get nobody to find the cause of this matter my lines of code where it stalls :
N89 G01 Z.556 F20.
N90 G1 G41 D4 Y1.5212
N91 G2 X-4.5015 Y1.6565 I.1449 J-.0051
N92 X-4.4667 Y1.6604 I.0312 J-.121
N93 G3 X-3.3186 Y1.8177 I.102 J3.5235 RIGHT at this line it will give an alarm I ,J or K not allowed on G02/G03 ,it will execute it as long as I dont have any values on my TOOL WEAR page , thanks , regards

Click to expand...

Rest assured that the Haas control is not at fault here.
IOW, if the movement is geometricly possible, then the Haas control will do it. ( likely a Fanuc, Mits, Siemens or Heidenhein will as well but that's not the question ...)

Please, post the entire code here as we have no idea where the tool is before block 89.