[allenp]

how to set tool diameter offset number on haas vf2?
I program on fanuc machines and they use T1 - H1 - D21 type compensations,
I'd like to use the same thing on haas so I don't need to change postprocessor every time I create program for different machine.

[djm77]

Can't remember which number it is and I'm not at work at the moment, but there is a setting for H+D to match up your tool number. You need to turn this off.


Sent from my iPad using Tapatalk

[Fletch_CNC]

If you turn off setting 15, the H and T codes don't have to match. There is no requirement for the D code to match. It's just a lot easier to keep everything on the same line in the offsets page if you use T1-H1-D1 etc.

[allenp]

ok thanks guys, also, do you know which setting it is to add a decimal point after each number you insert (without one) automatically?

but are you sure that setting 15 is what im looking for?
I already can use two diameters on same program, so for one part of milling there is D1, for other D11 on the same tool, with no alarm from machine.
I need to set machine to automatically measure tool to Diameter D21 in tool table, when i use renishaw auto measurement of tool length and diameter.

[Fletch_CNC]

A Haas can use whatever D value, there is no setting to restrict it to being the same as the tool number. Setting 15 (if it is on) means the H and T codes have to match. If you want to use a different H offset number, turn this off.

I don't know of a setting to allow you to have a decimal automatically entered for offset entry. Setting 162 will enter a leading decimal for you (that is, you enter X-2, and it the control will enter X-.0002). But that's not the same thing, and it applies to entering things in MDI or Edit mode. For offsets, numbers without a decimal are taken as being in tenths.

To have the tool diameter set to a different location by the probing routines, you would have to edit the routines themselves. They are designed to set the diameter offset of the current tool. You could write yourself a little program to move the values to the offsets you want to use, and just run that after you do your tool set ups.

[allenp]

i thought so but hoped there would be the solution.
i dont know why on fanuc there is only H table no D offsets.
so they have to use H1 as a lenght and H21 as "D21" so my postprocessor uses the same.
so now with haas i have to change postprocessor just to change D21 to D1, everything else is the same, which is stupid and annoying to me.

also, is there a parameter on haas which enables to choose how many decimals you can use on coordinates?
for example my solidcam post gives X-2.3233 and haas will throw an error "bad number" because it reads only 3 decimals.
how to change it?

[allenp]

back to the original question.
is there a way to change or make a custom routine for tool diameter offset entry while measuring?
the machine is new, under waranty, so I guess that wouldnt be possible without paying for a service visit.

also, is there a way to change the depth of tool contact with renishaw while measuring the diameter of tool?
asking because we've got a lot of small and short tools which have only 3-4 mm lenght of cut so it would be more convenien if z was 3mm deep on renishaw disk.

[haastec]

back to the original question.
is there a way to change or make a custom routine for tool diameter offset entry while measuring?
the machine is new, under waranty, so I guess that wouldnt be possible without paying for a service visit.

also, is there a way to change the depth of tool contact with renishaw while measuring the diameter of tool?
asking because we've got a lot of small and short tools which have only 3-4 mm lenght of cut so it would be more convenien if z was 3mm deep on renishaw disk.

Like Fletch mentioned, the way the routines are written the H number corresponds to the tool number. T1 H1, T25 H25. If you want T1 H71, then you will need to set it in H1 then copy to H71.

For both of your questions, it's possible that you may be able to edit the Renishaw macro's, but you will probably need to call them directly and ask their tech support. Their USA phone support has been great for me in the past, but not sure about Europe.

Good luck!

[Fletch_CNC]

You could always write a custom routine, too.The Renishaw programs aren't magic-- they're just complicated. But the heart of them is just using G31 (skip signal capture). Or you could write a program using G35-- that will allow you to use a different offset number, if you like.

I can't say for certain where in the programs it determines how far down to probe, but that can be changed as well. Now that I think of it, does the value in the offset table for Edge Measure have anything to do with how deep it probes? I would imagine so.

[allenp]

hmm interesting, can you add this new program for measuring tool diameter to the template haas came with?
the one you switch on when you turn on the machine (mdi - program - enter - f2 - select template - enter)?

so instead of using those scripts we could always use mine where the tool diameter is saved to +20 location? t1 - h1- d21?

[Fletch_CNC]

Yes, you can do that. You can write a routine to do most anything. The limitation of using G35 is it only measures the tool once, where using the probing routines touches the probe twice on each side-- a rough touch and then a finish. But if you set your touches at a low enough feed rate, it probably wouldn't matter. But to make it set a different offset than the current tool, you could just use something like : G35 F50. D[#3026+20.] There are example programs in the manual.

[allenp]

thanks!!
now please tell me how to avoid crashing renishaw? what do i need to take special care of?

[Fletch_CNC]

Well, in general, use subroutine 9810 when moving around-- that's protected positioning move. That's more for if you are movign the spindle probe from place to place. But it isn't a bad idea to use G31 M78 when moving around the table probe (like positioning the tool from one side to the other). That way, if you hit the probe when you didn't mean to (the touch off, at least), the machine will stop. Assuming you have turned on the probe. There's example programs in the manual, and in the Renishaw manual.

[haastec]

thanks!!
now please tell me how to avoid crashing renishaw? what do i need to take special care of?

Use the G9810 code as mentioned, but by far, the biggest reason for damage that I personally see is while manually jogging around.

The most frequent line I hear is "I thought I was in (blank) axis but I was actually in (blank), and I broke the probe, sorry."

This is what I always preach:

When jogging anywhere close to a part, jog in .001" increment. Yes it's slow, but you are not after speed here.
When jogging away from the part, such as after a routine has finished, start in .001 and very slowly crank the jog wheel and verify that you are going the correct way. Then when clear of the part good, go ahead and switch to .010" increment jog.
Go slow.
Be methodical about what you are doing.
Verify on the screen the axis selection prior to jogging.
Go slow.
READ any directions given on the screen.
Did I already say go slow?

Good luck!

[Fletch_CNC]

Did you mention going slow, haastec? That's a good safety tip. Oh, ok, you've got it covered!