A Fadal toolsetting system that doesn't suck!

Introduction:

These macros are designed to make the built-in Fadal fixture and toolsetting routines more useful. The default routines both want to output negative offsets (negative lengths for tools, negative Z axis fixture offsets) which means they don't ever meet in the middle like they should.

The default fixture offset system also does not account for the length of the tool being used to set the offset, so it will always be incorrect by the length of the tool unless you adjust it manually.

The macros in this package are designed to eliminate these issues and make working with the control much easier.

Benefits:

• Tools only ever need to be measured once
• Positive tool lengths measured from the spindle gage line
• Negative Z fixture offsets measured from the spindle face at the Z axis Cold Start position
• All measurements happen on the machine
• Tool lengths are portable and can also be measured offline using a presetter
• Ability to easily use a Haimer 3D sensor or other in-spindle measurement tool
• A wiggler, gage pin or simple electronic edge finder will work perfectly as well

IMPORTANT:
You need to have a reference tool in tool position #1. It doesn't matter whether this is an edge finder or something like a Haimer 3D sensor as long as its height and diameter do not ever change.

Summary:

Setup:

1. Copy the macros onto your control
2. Measure the distance from your spindle nose to the machine table at cold start
3. Put that value into V2 of program O9001 (toolsetting_macro.txt)

To measure your tools:

1. Run the Fadal tool length utility, measure your tool lengths using a gage block or tool setter on the machine table
2. Convert the tool lengths to positive values using the downloaded macro (Command menu -> Space bar -> press 0 for custom macro -> option 1)

To measure your fixture offset:

1. Make sure you have a reference tool in Pot #1, and that it has been measured for length
2. Measure all your fixture offsets using tool #1 and the Fadal fixture utility (Command menu -> 'UT' -> Option 1)
3. Compensate the fixture offset Z coordinate for the length of the reference tool using the downloaded macro (Command menu -> Space bar -> press 0 for custom macro -> option 2)

Installation:

There are 3 files that need to be copied to your machine:

1. ustom_macro_chooser.txt (Program #9999)
2. toolsetting_macro_.txt (Program #9001)
3. fixture_offset_compensator.txt (Program #9002)

Please note that the program numbers need to stay as stated for the sytem to work as expected.

After copying them the 'custom macro chooser' will be accessible from the Fadal quick menus (spacebar menu) by pressing 0 (zero).

Setup:

First thing we need to do is get a measurement of how far the spindle face is from the table when it's at the cold start position. I did this by stacking up some 123 blocks and my toolsetter to make a 5" tall gage, then lowering the spindle nose until it's touching the top of the gage stack.

At this point the Z reading is noted from the screen and then added to the height of the gage stack.

For example:

Note this number down. You then need to edit the 'toolsetting_macro.txt' to enter this number. The number should go on line 12 as variable 'V2' like so:


Make sure to replace the existing value.



Toolsetting:

Now you can go ahead and touch off your tools on a toolsetter that's sitting on the table. Using a gage block or 123 block is fine as well, just as long as you know the height. Using the Fadal utilities for this is easy and convenient.

Use the Fadal toolsetting utility to touch off all your tools. Touch off the tools on a toolsetter or gage block that is on the machine table.

• Press manual to get to the command prompt
• Type 'UT' to open the utilities menu
• Choose option 1 to enter the toolsetting utility
• Follow the onscreen instructions

After you have set the lengths of all your tools you should have a tool table full of negative values.

Now we can run the toolsetting macro to convert the negative values into positive values representing the overall tool length from the spindle gage line.

The macro does this by taking the negative values in the tool table and subtracting the machine's distance from the table to the spindle face at cold start that we measured during the setup process. For example:


The macros simply automates this calculation for any tools in your tool table that have negative lengths.

To run the macro:

• Press manual to get to the command prompt
• Press spacebar to get to the quick menu
• Press 0 to launch the custom macro
• Choose option 1 (CONVERT NEGATIVE TOOL LENGTHS TO POSITIVE)
• You will be prompted asking you if you would like to update your tools

After running the macro your tool table should be full of nice clean positive tool lengths.





Setting fixture offsets:


Now that we have our tool lengths (most importantly we have the length of tool #1, our reference tool) we can set a fixture offset.

Use the Fadal utilities to find the location of your fixture offset (X,Y and Z) using tool #1 as your reference.

• Press manual to get to the command prompt
• Type 'UT' to open the utilities menu
• Choose option 2 to enter the fixture setting utility
• Follow the onscreen instructions

The fixture setting utility will generate a negative Z value, but it won't be correct because tool length compensation is not active during the fixture location cycle.

To fix this we can run the fixture compensator:

• Press manual until you get the command prompt
• Press spacebar to get the quick menu
• Press 0 (zero) to launch the custom macro
• Choose option 2 (FIXTURE OFFSET COMPENSATOR)
• Enter the number of the fixture offset you want to update
• Confirm the change

This macro basically takes the Z value that's set in the fixture offset table, and subtracts the length of the reference tool to calculate the real Z position of that offset, for example:






Disclaimer:

THE TOOLSETTING MACRO MAY GENERATE MACHINE MOVEMENT!

Because of the way Fadal macros work (you can't have more than 16 consecutive lines with no machine motion) I have to jog the Z axis by 0.0001" every few lines just to let the program keep running. I'm doing this with 'G1 F1. G91 Z0.0001', and then moving it back to its original position after the program is done.

I don't believe this small movement should cause any issues, but just be warned and careful!

As always please use these programs at your own risk!

Download:

Download the latest version of the macros as a ZIP file from this link:


The macros are stored on GitHub to ensure they'll always be available.

Let me know if you have any questions or suggestions!

-Aaron

Aaron I've been following the threads about your Fadal very closely. I just got my own VMC 20 and as soon as I get the phase converter I'll post some pics of my install. I've made enough parts/money with my old Lagun mill w/Bandit controller to pay for the Fadal. I don't quite understand how to set the offsets yet, but this will surely help out. Thanks.

J. Clear

jjclear said:

Aaron I've been following the threads about your Fadal very closely. I just got my own VMC 20 and as soon as I get the phase converter I'll post some pics of my install. I've made enough parts/money with my old Lagun mill w/Bandit controller to pay for the Fadal. I don't quite understand how to set the offsets yet, but this will surely help out. Thanks.

J. Clear

Click to expand...

Sounds good mate, and congratulations!

Let me know if there are any parts of this post in particular that you don't understand and I will add extra information where I can! I would like this post to be a useful resource, especially for people like you and I that are just learning the control!

I don't deal with any Fadal's, but that's a very clear and descriptive write-up that will surely help some

If I had my own machine I'd be trying this right now. I'm fairly certain that work would be unhappy about a sudden change in workflow, though.

Someday!

Oh, and excellent work!

Nice, but kind of a lot of work. It's pretty easy to get a table mounted tool probe going on a fadal and get the same result using the l9101 routines or the UT menu.. But in the absense of that, good job. It's thorough and does a good job of demonstrating how the numbers can be manipulated to achieve different end results.

Rstewart said:

I don't deal with any Fadal's, but that's a very clear and descriptive write-up that will surely help some

Click to expand...

Thanks mate! Glad to know it comes across ok!

Atomkinder said:

If I had my own machine I'd be trying this right now. I'm fairly certain that work would be unhappy about a sudden change in workflow, though.

Someday!

Oh, and excellent work!

Click to expand...

Hey man!
Out of curiosity, what's the workflow at your work for tool and fixture offsets?

And thanks!

rlockwood said:

Nice, but kind of a lot of work. It's pretty easy to get a table mounted tool probe going on a fadal and get the same result using the l9101 routines or the UT menu.. But in the absense of that, good job. It's thorough and does a good job of demonstrating how the numbers can be manipulated to achieve different end results.

Click to expand...

Without having a probe I reckon this is about the least amount of work that can be done for a sensible solution.

With the probe obviously it's a different story... When using the tool probe on the Fadal does it put negative or positive values in the tool table?

I've been mucking about with the electrical interface for probing on my machine, I'm fairly confident that my $100 cheapo toolsetter can be wired to be a 'real' tool probe for less than $30 or so. Optoisolator driven by the battery in the toolsetter linked up to the input on the Fadal and you're essentially done. I've put that project aside for the sake of expediency for the moment, but it will happen in a while.

I'm keeping an eye out for proper renishaw probes and so on too though.

aarongough said:

Hey man!
Out of curiosity, what's the workflow at your work for tool and fixture offsets?

And thanks!

Click to expand...

Pretty abysmal. We make many of the same parts in very short runs over and over, and it's tons of "put vise on table, edge find stock corner, touch tools off, run parts, take vise off, put fixture on table, sweep in bore, touch tools off, run parts..." you get the idea. Our Haas VF-6SS has a Chick subplate on it, but so little work has been "ported" over and no one had ever taken the jaws off the One-Lok vises, so my next goal is start making softjaws and creating programs with specific locations. No more probing needed if done well, or possibly integrate probing into the beginning of the program. Most of our tolerances are fairly loose, rarely anything closer than ±.005" and 98% of those are clearance or fit diameters not heights. The Chick vises should repeat within a couple thou I think.

not sure why you would want to do it that way.
the CS position is easily established by just lining up the register marks for all the axises
the hit CS and it's done.
that is the reference point you need for the tool changer to work.

then load the tools in the changer pick some spot for your reference point.
and run the tool set utility. tool off sets are done
I use the top of the rotary table.
and use tool 21 for the reference tool.

one good reason to use the utilities is there is no fat finger error.

you know why reinvent the wheel

72bwhite said:

not sure why you would want to do it that way.
the CS position is easily established by just lining up the register marks for all the axises
the hit CS and it's done.
that is the reference point you need for the tool changer to work.

then load the tools in the changer pick some spot for your reference point.
and run the tool set utility. tool off sets are done
I use the top of the rotary table.
and use tool 21 for the reference tool.

one good reason to use the utilities is there is no fat finger error.

you know why reinvent the wheel

Click to expand...

I think you're misunderstanding what's going on here...

I'm not changing the cold start position, I'm using it as a reference in fact!

I'm also using the utilities for the tool setting and fixture setting. Nothing to be fat-fingered because everything after that is automated with the macros.

The setup stage where I measure the spindle face to the table is only ever done once, perhaps that's the part that's confusing you?

I added a summary to the top of the original post that should better illustrate how simple the process is when using the macros. I think that explaining it all in detail step by step made it seem way more complicated than it is.

The process literally takes seconds and is likely way faster than most other methods when using the macros. You only ever have to set tool lengths once which will save you a lot of time if you're currently touching off tools with each fixture change.

Well done Aaron and good pics, Using pos offsets and if a mistake is made in a program does the tool down or cut air? I use neg offsets because that is the way I learned. I touch off with my ref tool and away I go with any tools loaded in the changer. What are pro and cons of using pos offsets? Sorry about getting alittle off track.

Atomkinder said:

Pretty abysmal. We make many of the same parts in very short runs over and over, and it's tons of "put vise on table, edge find stock corner, touch tools off, run parts, take vise off, put fixture on table, sweep in bore, touch tools off, run parts..." you get the idea. Our Haas VF-6SS has a Chick subplate on it, but so little work has been "ported" over and no one had ever taken the jaws off the One-Lok vises, so my next goal is start making softjaws and creating programs with specific locations. No more probing needed if done well, or possibly integrate probing into the beginning of the program. Most of our tolerances are fairly loose, rarely anything closer than ±.005" and 98% of those are clearance or fit diameters not heights. The Chick vises should repeat within a couple thou I think.

Click to expand...

Well sounds like you've got plenty of space to introduce improvements then!

I'll be interested to see what you come up with!

twr said:

Well done Aaron and good pics, Using pos offsets and if a mistake is made in a program does the tool down or cut air? I use neg offsets because that is the way I learned. I touch off with my ref tool and away I go with any tools loaded in the changer. What are pro and cons of using pos offsets? Sorry about getting alittle off track.

Click to expand...

Main pros of positive tool lengths:
* Can be measured offline if you want
* Tools can theoretically be moved between machines
* Makes a bit more sense in terms of thinking about tool lengths

If you accidentally forget to convert one of the tool lengths then I *think* the machine should move up and away from the workpiece and either cut air or fault the Z positive limit. I will double check that tomorrow as trying to work out the behaviour in my head is probably not the best way of confirming that...

With the fixture offsets, if you forget to compensate the Z then again it should cut air (it will be the length of your reference tool above the work).

So overall the system should be fairly safe I think. I have to use it a bit more before I give my real verdict...

* Makes a bit more sense in terms of thinking about tool lengths
I can see this one the other 2 are not going to help me with only one machine and I don't have a bench tool length setup tool. The cutting air or tool going down I am interested in.

twr said:

* Makes a bit more sense in terms of thinking about tool lengths
I can see this one the other 2 are not going to help me with only one machine and I don't have a bench tool length setup tool. The cutting air or tool going down I am interested in.

Click to expand...

I'll get a definite answer for you tomorrow, pretty sure it should fault the Z axis positive limit as it tries to move up and away from the work.

The main reason I wanted to get a system sorted out was so I could use the Haimer for fixture offsets, and so I could measure tools once and forget about it. This system should accomplish both and will save me a lot of time I'm sure!

Im Lost Not hard to do sometimes LOL) I do not get the need for it. I have a heidenhain control so that maybe the difference. I do use the hiemer for offsets thought. Once I change the offset all my reference tool is zero and tool lengths are now based off the new offset. Are you saying that the way fadel does it you have to remeasure all your tools for each fixture offset. If so that sounds really odd to me. FYI Im very jealous of your programing skills I would love to know more about macro's.

B-Mathews said:

Im Lost Not hard to do sometimes LOL) I do not get the need for it. I have a heidenhain control so that maybe the difference. I do use the hiemer for offsets thought. Once I change the offset all my reference tool is zero and tool lengths are now based off the new offset. Are you saying that the way fadel does it you have to remeasure all your tools for each fixture offset. If so that sounds really odd to me. FYI Im very jealous of your programing skills I would love to know more about macro's.

Click to expand...

Hey Brett!
Remeasuring the tools each time is not something that's inherent to the Fadal, just the way some guys use it.

The reason I had to write the programs is mainly because the Fadal fixture offset cycle does not account for the length of the reference tool. So if I use my haimer to measure the z offset it will be incorrect by the length of the tool. Also because the tool setting cycle and the offset cycle both want to output negative numbers they don't really meet in the middle as far as I can see.

I think the tool setting cycles on the control are optimized for probing rather than manual measurement. Of course I might be totally missing something, but I tried for a while to get the default setup to work, as well as reading a bunch of different manuals and guides before concluding that it simply didn't work in a reasonable fashion.

With the addition of the 2 macros though it actually works out to be very nice, quite convenient. Not as convenient as straight automated probing, but fairly close.

I actually really like the haimer, being able to sweep a face with it is a big advantage over a spindle probe. Not that I would turn down a spindle or tool probe if they came up