Old Haas with version 8.8 control problem with tool offsets

Hi Guy's,

I have ditch my crappy Chinese bench top mill and bought an old VF-0. After a month sorting out electrical issues its now running :-)

The control has some 1999 (8.8) vintage software with the quaint old CRT display. I have loaded tools and attached a vice and an making so initial attempts to program it.

I have followed the manual and am making a fixture plate with about 50 odd holes.

I have followed the setup procedure in the manual and touched off all the tools using tool hight and next tool buttons to the top of the stock.

I then set G54 origin to the top left of the stock. Then I uploaded the G code from Solidworks / CAM Works with the free 3 Axis Hawk Ridge Haas Post processor.

Pushed the 5% Rapids and cycle start.

Managed to go through 4 lines of Code and spat the dummy when it got to the G43 H3 Z10. Z Axis travel out of range.

Looking in the Haas manual this code is what's suggested.

If I add in some basic code via MDI to drill a couple of holes and don't apply the tool height offset with G43 the tool offsets seem finer and I managed to drill 4 holes using the G83 canned cycle no problems.

Anybody know what Im doing wrong?

your Z value with the g43 should not exceed 1 inch , is the controlset to metric?. also what does parameter 57 say on negative offsets. I run mine on negative offsets as it's the easiest setup to program with. if it is negative, your offset Z values of your tools needs to be a negative number. also make sure you have no values on g52 and g92 on your offset page.

Hoss,

Yes my controller is set to metric as Im in the UK. I will check in the morning, but I'm sure my tool offsets are negative values. I assumed these where machine values with no work offsets applied as all z moves are negative. The G43 H06 is 35mm so over 1 inch so you may be on to something! Why is there a limit of less that 1 inch? I assumed the whole line G43 H06 Z35. M08 was to lower the tool to the R plane in preparation to start drilling canned cycle. The next row is G82 G98 R3. Z-20. P1. F45.989.

Thanks Again,

Ian.

slipalong said:

Hoss,

Yes my controller is set to metric as Im in the UK. I will check in the morning, but I'm sure my tool offsets are negative values. I assumed these where machine values with no work offsets applied as all z moves are negative. The G43 H06 is 35mm so over 1 inch so you may be on to something! Why is there a limit of less that 1 inch? I assumed the whole line G43 H06 Z35. M08 was to lower the tool to the R plane in preparation to start drilling canned cycle. The next row is G82 G98 R3. Z-20. P1. F45.989.

Thanks Again,

Ian.

Click to expand...

So I checked and tool offsets negative is set to 1. As an example tool 6 has an offset of -287.640mm
G54 Z offset for the stock top is -281.5mm
When I do a G43 H06 then the work Z figure went to 535 mm and threw an z axis out of range error.

If I delete the G43 lines then its seeming to act as expected. I know on my old Linux cnc and Tormach controls I don't remember using G43 as I think the offsets automatically took effect after a tool change.

Thanks,

Ian.

so is it traveling + towards Z home or negative as in going thru the part ? also what is you value on Z of your g54? where are you touching the tools off from ?

Hoss,

G54 Z offset for the stock top is -281.5mm. That was done with the part set zero button.


the movement of the z is as I expect with + moving up and away from the part and any minus numbers moving into the part. If I MDI G54 and load a tool then X0 Y0 Z10 the point of the tool moved 10mm above the origin as you would expect. No G43 necessary??

Had a brain wave and looked at some of the programs that I backed up to disk that where on the control when I got it. Opening few lines for you perusal:

O0009
(CRANE OPP3.NC)

M31
T10 M06
(T7 - 12MM EMILL)
G90 G80 G40 G54
S2200 M03
G43 H10 / M08
G00 X-81. Y-35.25
Z10.
Z2.
G01 Z26.7 F1000
Y35.35 F800
Z2.


And no the backslash wasn't a typo :-)

Thanks,

Ian.

if you are touching the tools off of the top of the part. your g54 Z should be set to 0. if you're using a Joe block off of the table and the part is above the block the you enter the measurement from Joe block to top of part in a + positive number.

Hoss710 said:

if you are touching the tools off of the top of the part. your g54 Z should be set to 0. if you're using a Joe block off of the table and the part is above the block the you enter the measurement from Joe block to top of part in a + positive number.

Click to expand...

That's exactly the way I do it.
Think of it this way: the G54 Z value is just the difference between your tool touchoff point and your refenced part zero plane (or top of part). For example; touch off is using a 50mm block off the table. The top of the part is 150 mm above the table. Your G54 Z value should be 100. Note, positive not negative.) I think what you are doing is hitting the part zero button at the Z zero plane. DON'T DO IT!

Before you set your Z offset, you should take a tool and touch it off at, in this case 50 mm off the table. Then, in the tool page press the Set Tool Height button. This should put in a value that matches the current Z position of the G53 machine offsets, a negative number like -400.

slipalong said:

So I checked and tool offsets negative is set to 1. As an example tool 6 has an offset of -287.640mm
G54 Z offset for the stock top is -281.5mm
When I do a G43 H06 then the work Z figure went to 535 mm and threw an z axis out of range error.

Ian.

Click to expand...

^^^^ There lies your problem!!! ^^^
Basically your toolsetting process is incorrect.

What you are asking the machine to do is to make a 568 mm move!!! It does not have that much travel!!!

The problem with your toolsetting process is simple: IF you are using the top of the part to pick up the tool heights, then the Z value in G54 should be 0!
IOW
You don't set the G54 Z plane by entering a value in the "Workoffset" page, rather you're telling the machine that for Tool1 it needs to travel "N" distance to get to the top of the part
and that value is set in the "Tool Length Offset" page!

Remember, the Z travel is ALWAYS the sum of Tool length offset + Workoffset Z + G52 Z!

With that said, there is a much much better way to set your tools up, but please let us know if you undersood what I wrote there!

Hoss710 said:

if you are touching the tools off of the top of the part. your g54 Z should be set to 0. if you're using a Joe block off of the table and the part is above the block the you enter the measurement from Joe block to top of part in a + positive number.

Click to expand...

Yes That was the problem. I was touching off on the part and I had a Z offset for G54. Doh!

Thanks for the assistance!!

Regards,

Ian.

Yes made sense. My old Tormach worked differently. I was able to touch off all the tools and then put a different job in and just re-touch one tool to the top of the new setup and and it adjusted all the tools.

It will get a bit boring touching off all the tools every time I change job. Im not running in a production environment, more of a job shop so different work every day.

Thanks,

Ian.

slipalong said:

Yes made sense. My old Tormach worked differently. I was able to touch off all the tools and then put a different job in and just re-touch one tool to the top of the new setup and and it adjusted all the tools.

It will get a bit boring touching off all the tools every time I change job. Im not running in a production environment, more of a job shop so different work every day.

Thanks,

Ian.

Click to expand...

You can do that on a Haas as well, but it's likely different than the Tormach.

If you have the book, look into setting #64: "T OFS MEAS USES WORK"

If you set it to OFF, then the tool setting procedure changes somewhat.
Instead of setting your tools to the top of the part, you will be setting it to a fixed point on the table. Any fixed point, as long as it remains consistant.
Most of us typically use a gage block or gage pin on top of the back of the vise or a corner of the table, but it's all up to you.
Jog to this block with all your tools to touch, and hit "T Offset Measur" for each.
Then to set up the workoffset, take an indicator in a toolholder, jog to the block until the dial reads 0 and the zero the OPERATOR coordinate.
Now jog over to the top of your part ( or wherever you want your work Z0 to be ) jog down until the dial reads 0.
The take the value in the OPERATOR screen and enter it in the appropriate workoffset Z field.

Basically what you're doing is you separate the tool heights and the work offsets, none of them depends on the other, rather they both depend on a single fixed
point in the work envelope.
You will be setting the tools from HOME to the block, and the workoffset from the block to the part Z0.
This way you can use any workoffset with any tool at any time, and you can delete any tool and any workoffset at any time without affecting anything else.