Speedio s700x1 Tool Height Offsets (and Haimer 3D Taster) - Confusion

[jehake12]

I'm having problems with my z axis position on my speedio s700x1. I have not made a part on it yet.

I set a haimer probe on my speedio in T20.
I set the tool length offset for T20 to 5.2XXX" (in data bank --> 2. Tool Data --> 1. Tool List --> T20 Tool Length Offset )
I jogged the spindle w/ T20 loaded such that the Haimer zero'd out.
I set the work offset with the spindle in the haimer position above. (data bank --> 1. Workpiece coordinate zero --> G54 --> automatic setting w/ 0.000 adjustment for x, y, z).

I switch to my T4 with tool length offset to 3.7XXX" using the ATC buttons and rotate L/R.
I jog to my absolute position from above.
I see the tip of the endmill is about 1.5XXX" above my G54 position.

I was expecting the speedio to compensate for the different tool height when I changed tools, but it did not do this in manual mode. Is this normal? Am I doing it wrong?

I tried to cut a simple part. The CAM program uses a G43 H04 for tool height offsetting the T4 from above.
When the speedio goes to make the first operation, the endmill is about 5.2XXX" above the G54 position.

What am I doing wrong?

Thanks for any help.

 

[finix]

When setting your G54 Z offset, call your Haimer tool T20 with G43 and its relevant H value this case H20. Then redo it again and it should check out. I haven’t use a manual probe in awhile but I think that is where you are running into issues. Did you come from being used to Heidenhain by any chance?

 

[Pete Deal]

Here's what i do.
My Haimer is set as T99 always. It pretty much lives in position 21 in the tool carousel.

To do Z probing with it I enter the following line in MDI mode-
T99M6G54.1P47G45H99Z9

This line sets the tool at 9" above the table then I can go ahead and manually jog it around and measure Z. I have the extended coordinate P47 is set to X=0, Y=0, Z=0.

The machine seems to default to coordinate system G54 so I specify the extended coordinate P47. I tried to setup a macro to do this but once the macro ends it goes back to G54. There's probably a better way but I haven't found it yet.

Also, I just recently bought one of the super short 3/4" tool holders from Maritool for my Haimer. This is the shortest way I have found to hold it. It's nice for 4th axis stuff.

 

[13engines]

Is this machine using a Brother overlay on a Fanuc control?

I'm having problems with my z axis position on my speedio s700x1. I have not made a part on it yet.

I set a haimer probe on my speedio in T20.
I set the tool length offset for T20 to 5.2XXX" (in data bank --> 2. Tool Data --> 1. Tool List --> T20 Tool Length Offset )
I jogged the spindle w/ T20 loaded such that the Haimer zero'd out.

I set the work offset with the spindle in the haimer position above. (data bank --> 1. Workpiece coordinate zero --> G54 --> automatic setting w/ 0.000 adjustment for x, y, z).

When you say you "set" your T20 to 5.2XXX and it was "zeroed out", it appears from your comments that you were at the Z zero position of your current part. Meaning the Z reference surface you programmed to in CAD/CAM. Is that correct?

If so, where did you get the number 5.2XXX? Let's hope it came only from the Machine Position Display. And why is it not a negative number?

I switch to my T4 with tool length offset to 3.7XXX" using the ATC buttons and rotate L/R.
I jog to my absolute position from above.
I see the tip of the endmill is about 1.5XXX" above my G54 position.

Now with T4 also on the part surface, where did you get this 3.7XXX number from? And again, why is the Tool Offset number positive and not negative?

Can you explain the type of Offset System you're trying to use? Seems like #4.

1) Master tool? (Always a non zero Z setting in G54)
2) Repeatable at any time Setting Master? (Always a non zero Z setting in G54)
3) Offline? (Always a non zero Z setting in Work Offsets)
4) Current part programmed Z0 Surface? (Z work offset always zero.)

I was expecting the speedio to compensate for the different tool height when I changed tools, but it did not do this in manual mode. Is this normal? Am I doing it wrong?

I tried to cut a simple part. The CAM program uses a G43 H04 for tool height offsetting the T4 from above.
When the speedio goes to make the first operation, the endmill is about 5.2XXX" above the G54 position.

What am I doing wrong?

Thanks for any help.

We'll get to this later.

 

[jehake12]

The machine has the brother C00 control.

The CAM for the part had G54 Z zero set to top of stock. (Top face, left face, back face of stock is my G54)
To teach the machine where G54 Z zero is, I set the Haimer probe to top of stock until it reads zero on the Haimer gauge.

The tool length offset from the spindle gauge to the tip of the haimer was established using a 1-2-3 block. There is a tool height setter on the machine which was used to set T04 TLO to 3.7273". So one of the tools had a known tool length offset from using the tool height setting function. Then I slid the 1-2-3 block under the tip of the known tool to determine machine z height. I did the same with the heimer probe. Then I solved for the unknown haimer offset for that given 1-2-3 block:
(Machine z known tool) + (known tool off set) = (Machine z haimer) + (unknown haimer off set).

This set the Haimer TLO to 5.2686" on T20.

When I'm on manual conditions window, I was expecting that Absolute coordinate positions would show the XYZ position for the current bottom tip of tool in the spindle pulling the TLO parameter from the data bank. It seems to always show the exact same XYZ position regardless of any TLO in the data bank. T1-T20 all read the same Absolute coordinates. This occurs if I use the ATC and turret rotate keys on the user interface or the T##M06 command on the MDI. When I set the Z for G54 on the machine, I could have subtracted out the 5.2686" for the haimer offset manually and that would probably let my test part cut. However, I would like to see the Z position for the tip of whatever tool I have showing up in the absolute coordinate position window. Maybe I'm not thinking like a machinist and no one really needs that info from the Abs coord position.

Attempting to use ----> 4) Current part programmed Z0 Surface? (Z work offset always zero.)

Thanks,

 

[13engines]

If I follow this correctly, you've managed to input an Offset for the Heimer that when theoretically zeroed on the in Machine Height Setter, it would read 5.2686. But again I ask, why isn't this a negative number? Not in every single world, but generally, Tool Offsets are negative numbers, and represent the distance the machine head has traveled in the Z minus direction from its Home Position, to whatever reference you've decided to use. In this case, the in machine Height Setter.
By having a Tool Setter in the machine, you are set up to use Offset Style #2 above.

Measure every tool for a job using the height setter. If there is a measure function on your machine, it will in some way reference the Machine Position. When measuring tools, make sure there are no active Z settings in any Work Offset, or they can lead to improper numbers being set. Once all tools are measured, take the Heimer and zero it out on your part Reference Surface. Then take the DIFFERENCE between the current Machine Position reading and the Tool Offset reading of the Heimer, and set this number in the G54 Work offset, or whatever other offset you happen to be using for the current work. Depending on the height of the workpiece compared to the height of your Setter, this Z setting may be Negative or Positive.

You're right in that there's no real reason to be concerned about the Absolute Display, but if you must, you have to have the Tool Offset active for the Absolute Display to read true. Meaning G43Hx has to be called. There was a thread on here recently that someone was trying the same thing you are in MDI. (Fanuc machine) Nothing wanted to work in MDI but worked fine in Auto or Memory mode. You might try that yourself.

If there ever was a display to be concerned about it will be Distance To Go. Most of what you really need to know is found there.

Wish I had some experience on a Brother control and it's resident Tool Setting Functions. My thoughts might be more directly relevant.

 

[hi-fly-cnc]

Hi, as others have summarised in different ways, the Brother control DOES NOT apply G43 height offset on tool change. YOU need to request it. Further, you cannot do a plain G43Hx, you also need to add a Z value. This is a bit annoying, but not the end of the world.

The thing you need to be wary of is manually doing a G43 from the MDI and having the tool crash somewhere you didn't expect because of that Z value being in a WCS that wasn't expected...

You could write a macro to do the tool change, apply the G43, ensure it doesn't actually move by doing the maths to offset current position by tool length... But.. You can't run macros (with params) from the MDI on the C)) control (grr). So you end up reduced to either setting the param in a memory location (set this on the hotkey), or setting them in a program, which you then edit/call.

There is a user setting to make it so you always edit the current program. This makes hopping back/forward between edit/run much faster.

I've got a Blum toolsetter and spindle probe, so no explicit experience with the process via a Haimer.

 

[Pete Deal]

The thing you need to be wary of is manually doing a G43 from the MDI and having the tool crash somewhere you didn't expect because of that Z value being in a WCS that wasn't expected...

This is why I always insert a "G54.1P47" in my mdi command line to make sure it's got a dedicated work coordinate. And then it's wise to set rapid override down when doing this incase of a typo.

 

[Peroni]

Our S700X1 has neither a tool setter or spindle probe. I use a Tschorn version of your Haimer plus a Tschorn manual tool setter. The latter's 4" height is compensated automatically via user parameters, switch 1 par 007. The vise bed is my reference and where I set all my tools and Z heights from.

I'll manually bring the indicator down to the vise and zero it, then I'll zero out the Z on machine display. From there I would measure the distance to wherever my program's Z zero point it. Be it parallel height, height of a fixture or stock. I'll manually enter that number from the machine's Z display into the G54 or whatever offset number I'm using. I only use automatic setting for X, Y and tool height and the machine does not need to know how long the indicator is.

 

[hi-fly-cnc]

And then it's wise to set rapid override down when doing this incase of a typo.

I think this advice is applicable generally whenever operating this machine with its bonkers acceleration...!!

 

[jehake12]

Thanks guys. Everyone was saying about the same thing.

I think Pete Deal's solution is the most ideal for my scenario.

I appreciate all the help!

 

[hi-fly-cnc]

Not totally related, but a relatively unknown tip is that if that you can reference a tool pocket by adding 100 to the pocket number. So if you want to quickly load whatever is in pocket 21 and you cannot remember the tool number, you can do an M6T121

 

[Eleven71Cutters]

already stated but your control does not automatically put in the H20 compensation for your Z height, although it does for your X/Y because the Haimer XY 0 is half the ball Diameter. if you walk it down until is zeros out and do the automatic set for your Z, you will need to subtract H20 from your WCS Z because it is going off your Spindle face, not the tip of your Haimer.

 

[BROTHERFRANK]

something you can do when running a taster, is you enter the length of the taster in the External Work Coordinate value. Same page as G54-G59. this value will be negative. To activate the External Work Coordinate you need to add a jumper to an external input on the IO board and map that input to EXWORK. When you touch off a surface with your taster, you will hit Auto Set. The value will be the work offset plus the taster length but the External Work value will automatically subtract it out for every work offset. This will make your work offsets appear larger but get you where you need. an easy test is to put 6" of gage block (1-2-3 blocks...) on the table. Bring you taster down on it and set a work offset. The value should be 6" plus the taster length. So if your taster is 5.233", the value in the Z Ext Work offset will be -5.233 and when you set a work offset (eg G54) with a 6" block the value should be 11.233.

 

[hi-fly-cnc]

something you can do when running a taster, is you enter the length of the taster in the External Work Coordinate value. Same page as G54-G59. this value will be negative.

Hmm, that's an interesting use of the External WCS!

I mostly use the External for dry run machining. If anyone has a Brother and DOESN'T have the external wired up, then I would strongly recommend it, it's quite useful! (I haven't ever used it for shifting an offset in X/Y, but I speculate there could be uses for nudging something in to a fixture position?)