I'm currently trying to use a centurion 6 control but I'm being met with some resistance. I can set the Z value for any of the work coordinates but it doesn't account for the Z value when say 'G55' is called. no matter what the value of Z in G55 or G54 or whatever, it doesn't change where the tool goes.

I'm trying to run this in MDI, simply trying to make the tool come 1" above the work.

G55G90G0X0Y0
T4M6
G43H4
G1Z1.

Any suggestions?

Tarkus,

G54-G59 are for X and Y work offsets and Z is always global. At least on the Milltronics as far as I know. In the hdw screen the wrk softkey goes away when you are moving in Z.

Is this any different on other mill controls?

DC

Almost every other mill made allows for a Z offset. I wish I didn't have to set my tools every time I set up a job. It'd be nice to just change the work offset and be able to keep the tool offsets.

Well, if you go into the utility screen and set the offset for say tool 2, 3, 4 etc, you can set tool offsets. Or you can use Z-tool in the the jog and hdw screens to set it.

To clarify what I meant was that G54-G59 do not change the Z as set up in the tool offset library.

DC

How do you set the Z height, say you have a new workpeice, without resetting all of the tools off the top of the part?

Lets see.

You could place tool 1 in the spindle and move it to Z0, then drop the knee(oops! if you have a knee) to set tool 1 on top of the part new part. Everything else would be relative to that.

Using G92 Z1, that shifts all work coordinates to the new value from where the machine is at, but it is a bit dangerous if you forget to cancel that. I do not know if that will mess with the soft limits the machine tracks. You would still place tool 1 on top of the part.

The manual states to cancel tool length offsets, but that won't help your use. G52 is similar.

Do you have a manual?

DC

From Main Screen Goto
Params
Coords
Select The Work Coordinate You Are Using And Change The Z Value There.
This Will Change The Offset For All Tools That Have Been Already Set
Hope This Helps

I just found that section in the Centurion 5/6 book. I had been looking at a Centurion 1 darndit!

This can also be done with a G10 but then you need to use the parameters like P414 etc. to make those changes in MDI. Which proves it can be done in several methods, but the book also shows in those several places that changing the Z plane is not recommended.

DC

My RH 30 has 20 pocket tool changer and when I change Z offset on G 54 cordinate page it causes the tool changer to not line up properly with the spindle. Milltronics offers a tool setting probe and software to do what you want to. another option is to go to parms/tools or on older software it is D or H offset and change the height of each tool by the Z height difference. The very safest is to teach each tool on each job because the few minutes it takes to make sure is a lot shorter than scrapping a part, tool holder,or possibly jamming your spindle into the table. A long long time ago when I was a lot younger and thought that time was money I looked for every short cut I could find. In the end a safe, conservative,approach to the job saves tools and equipment, time from changing prematurly dammaged or broken tools. In theroy it is a CNC it should be programmed to be able to be operated unatended and not have to be baby sat to get to the end of the job. at the end of the day you may not have as many parts, but the ones you do have are all good and your carbide expense is not going to break the bank. The Farmer.

Some controllers do not read more than one gcode per line. Might be worth a shot. Otherwise, I can't see why it would behave as if the Z value from the offset register had no effect.

Ok, I’ve followed this thread with interest because I feel every machine should be able to reset all tool lengths with just one command. But if I understand Farmers Machine that it can’t be done without effecting the tool change position, then again from what LYN BYRD he’s saying that it can be done in the params/cords menu. So who is right? If the Milltronics/Centurion can’t do this then Milltronics machines have a distinct disadvantage over their competitors. I would love to just set all tools to one location (2” above the table for example) and then inter the work piece’s Z location in one place, one time. I make dozens of setups a day and need to streamline the process.
Has any one tried what LYN BYRD suggests? Can anyone confirm what Farmer Machine experienced?

I look forward to a solution.

Ok, I’ve followed this thread with interest because I feel every machine should be able to reset all tool lengths with just one command. But if I understand Farmers Machine that it can’t be done without effecting the tool change position, then again from what LYN BYRD he’s saying that it can be done in the params/cords menu. So who is right? If the Milltronics/Centurion can’t do this then Milltronics machines have a distinct disadvantage over their competitors. I would love to just set all tools to one location (2” above the table for example) and then inter the work piece’s Z location in one place, one time. I make dozens of setups a day and need to streamline the process.
Has any one tried what LYN BYRD suggests? Can anyone confirm what Farmer Machine experienced?

I look forward to a solution.

I run 2 milltronics cent 6 and you can set g54 g55 etc z offsetes just like fanuc and other controls (go to cordinate work choose cord set z value enter key)
simple
Bill

Bill,
That’s about is about as clear as mud. What menu are you referring to? Is it the one under parms-cords, then curser down to:
“WorkCoords 1 (G54) Subset 0 …….***” ?

We use the work coordinates under the parameters menu. You can successfully set different Z heigths there.

We use the work coordinates under the parameters menu. You can successfully set different Z heigths there.

I do this too. It causes no problems with tool change height, that is specified in machine coordinates.


Cheers
Dave

The tool change height is another parameter I believe in the same menu.

hi there, I think you might need a feed rate with a G1, a G00 dosent use feed rate but uses the machines rapids

hi there, I think you might need a feed rate with a G1, a G00 dosent use feed rate but uses the machines rapids

I use a Centurion 6 control. I always set my tools with a setting light that you can buy anywhere for under $100. I set the setter on the back stationary jaw block on my kurt vise. I set all my tools off of that setter. Then I measure from the top of the setter to the top of my part and go to F7 Parameters, F2 Coordinate, scroll down to G54 and press the edit key. Scroll down to the Z coordinate and enter that measurement in the Z offset and make sure to press enter. Watch your signs, + or -. Then I call the offset after the tool change and tool height command

T1M6
S3000 M3
G43 H1
M8
G54
G0 X0 Y0 Z.1

Works every time for me.
Ken

Finally the voice of experience gets it right!

You must make sure that in the g54 coordinate edit screen Z is zero before you set all your tool offsets. Set all your tool offsets (H's) first then change the G54 Z coordinate. If you run a program then decide to add another tool, change your G54 Z back to zero then the set the new tool offset (H), then change your G54 Z. I always use a 2" tool offset guage so my G54 Z is always zero when setting tools and -2.0 when cutting.