Heidenhain TNC 151 , series 1 Bridgeport

First let me re introduce myself Ive been on the forum since 2003, I cant remember the last time I posted. I have a new position as a Machinist/Instructor in a college with old equipment.
The problem is the; trying to run any program I get LIMIT SWITCH Z+ error, I have tested the switches all are working & restarted the machine several times.
Any Ideas?

Tool said:

First let me re introduce myself Ive been on the forum since 2003, I cant remember the last time I posted. I have a new position as a Machinist/Instructor in a college with old equipment.
The problem is the; trying to run any program I get LIMIT SWITCH Z+ error, I have tested the switches all are working & restarted the machine several times.
Any Ideas?

Click to expand...

Check the parameters, the Z+ is probably set wrong.

my R2C3 is set as follows:

MP 44 : +457,327
MP 45 : -1,270
MP 46 : +304,928
MP 47 : +0,000
MP 48 : +2,000
MP 49 : -127,127


44,45 are x
46,47, are y
48,49 are z

in mm, allowable travel from the zero encoder pulse.

If it is an Interact, the y will be different. it homes in the opposite direction

the numbers are to give you an idea of the appropriate range, all the machines have their own numbers


the heidenhain does not limit switches per se, it has a Z+ trip dog, which if it is electrically stuck, will cause the z to move down during homing, then the first encoder marker pulse it sees is zero. The trip dog is very close to Z+Max, so if this switch is sticking it will have little to no movement in the up direction, and will eventually hit the actual Z- limit switch. Hitting any of the actual limit switches will result in an EMO and you will have to move it off manually


The other thing that could be happening is that you have your Z set incorrectly. If you have Z zero set as the very top of the travel, you will have travel available only by programming -Z numbers, as you can see, my machine will give that error if you program any positive Z number larger than 2 mm, if it was zeroed at the topof travel

MOD
code number
95148
show you the parameters

download them immediately!

BTW I have a conversational fusion post that give a compact enough output to run programs on that machine....

Oh, and there are soft limits that are user resettable, I never use them and forget about them, also visible in mod

Only when running a program in run mode? How about dry run? Please elaborate on when it happens and under what conditions.

If only in these two modes, lower the knee to accomodate the needed travel and reset the Z reference. See Gustafson's last paragraph.

Thanks for the quick response. I've gotten really busy this week I didn't have much time to work on this issue but I did check all the MP setting and found everything to be as it was according to my manual and it doses this on all programs including dry cycle.

After all that I found it's something to do with my new post processor from bob-cad it works fine for drilling programs but not milling. It has no excessive z moves but something is wrong, I'll get back to it next week.

Thanks everyone.

Tool said:

After all that I found it's something to do with my new post processor from bob-cad it works fine for drilling programs but not milling. It has no excessive z moves but something is wrong, I'll get back to it next week.

Thanks everyone.

Click to expand...

I had a Fusion post send my 151 up into the limit switch, which basically should never happen

So, yeah, that can happen....

thanks everyone for the help , for 30+ years I worked with a groups guys and we could bounce problems and ideas off each other, now I work alone it's good to have this forum.

Thanks, Tool

The 151 (or at least my 155, which is the same with graphics) doesn't have work offsets in the traditional sense, so make sure that the code being generated isn't driving outside the travels (as the tool and coordinate system are presently set)

Also, make sure you're using M25 to retract the Z for tool change, not some sort of blind driving move.