What's new
What's new

Fadal VMC 3016FX CNC MILL

bigdon26

Plastic
Joined
Sep 14, 2017
I am new to the Fadal CNC mill. I am use to Mazaks.

My question for anyone & everyone is can I teach all my tools 4.000 off the machine table and use the G54,G55,G56 for my program "Z"? I want to standardize my 21 tools for all jobs and just teach a "taught tool" off the top of a part for my program "Z". Do I still use a G90 or do I use a G92 in my program?

I really could use the help. I am new here and the only machinist............
 
What do you mean by "teach all my tools 4.000 off the machine table?" Do you mean dry-run your program with an extra 4" on the Z work offset:? Sure. But, your control may have that sort of thing built-in -- is there a "Dry" button on the control?

If you mean something else, then I got nothing :scratchchin:.

Regards.

Mike
 
No I meant as a standard for all tools. Currently I'm have to teach all tools off the top of the part. Next job, I have to reteach the same tools of the top of the new part. So I wanna just teach my tools once and use them on every job without having to reteach for every job or different parts.
 
So, you want all your tools to be 4" long? Trust me, you don't want that ;).

You measure and store the tool lengths in the control, then you simply tell the machine which tool length to use in your code:

G0G90G17G40G64G69G80
G55G100T4L3X.3063Y-.3434S16000M3
N4G43H4Z.25

Regards.

Mike
 
So, if you set all your tools to a known height (like a 4" inch block off the table) in the machine, then your fixture height offsets (G54, G55, G56, etc..) are just the difference in height from that point.
 
No...
I'm saying now I bring my tools down to top of the part and (teach them) by using "length set" T4 H4 H14 H24

My G54 Z & G55 Z & G56 value are zero. So I bring my tools down to the top of the part and press "Length set" it come up with
H4 Z-10.3681
H14 Z-8.6578
H24 Z-7.9615

On a Mazak I would teach T4 H4 4.000 of the top of the machine table and then teach the G54 G55 G56 "Z" off the tops of the parts so on the next job I would not have to reteach T4 H4 again on the G54 G55 G56 "Z" off the top of the new part.
 
I think you're doing it backwards (although there are lots of ways to skin this cat ...).

1. Measure the gage length of all your tools, once (until you have to change out a cutter that is). These tool lengths don't change when your part height changes.
2. When it is time to make part #1, measure the height of the part.
3. Use all your tools, referencing the pre-measured tool lengths.
4. When it is time to make part #2, measure the height of the 2nd part, no need to re-measure tools.

With the method you describe, you are totally losing the utility of G54, G55, G56, etc.

Regards.

Mike
 
I guess I am just going to have to experiment.......

I don't know how else to explain this I only want one tool length for that tool on the machine and not every job!

Tool 4 is a 1.000 spot drill I have to use T4 H4 H14 H24 and I don't want to. I want to use T4 H4 for all three vises with the three different heights of my parts. By using the G54 G55 G56 Z values
 
I guess I am just going to have to experiment.......

I don't know how else to explain this I only want one tool length for that tool on the machine and not every job!

Tool 4 is a 1.000 spot drill I have to use T4 H4 H14 H24 and I don't want to. I want to use T4 H4 for all three vises with the three different heights of my parts. By using the G54 G55 G56 Z values

I am in strong agreement with you! The sequence I describe does this for you. Tool lengths are expressed as "gage length" which is the distance from the spindle nose to the tool tip. It is independent of part height. G54, G55, G56 are describing locations of various zero points, which can all be used interchangeably within a program, using the same tool gage lengths.

Regards.

Mike
 
The way I have found for getting running quickly on a Fadal is to ignore the Z value offsets in the work coordinate systems (G54, G55, E0, E1, etc..) and only set X and Y offsets in your WCS. Let Z remain at zero within all the WCS.

I set tools similar, with a block off the table, so after each is loaded it will be modified to account for the block height (typically done all at once with Mass Modify, after loading all tools). With this, Z zero is the table surface.

Next.. just use the Mass Modify function for all tool length offsets at each setup, based on the desired Z height from the table.

One handy trick to remember what the last 'mass Z' offset, is to offset one additional tool beyond what you have loaded. For example, I have a 21 tool changer, with 21 loaded, but I always do the Mass Modify through tool 22. For the next setup, I first mass modify all tools by the inverse of the tool 22 offset to get me back to zero Z offset.

This method certainly has its limitations, but works great for me when only doing one setup at a time. It keeps its simple, which I find is a good place to start. Good luck!
 
If your set all your tools to a standard height in the machine (whatever that may be), then each of your fixture height offsets (G54,, G55, G56, etc...) will be the difference in height from that point.

For instance, at our shop, tools are set to a 1" block at the bed of a vise. Our programs are written to have Z0 be the top of the finished part. So, if in my first vise (G54) I was going to make a 3" tall part, my second vise (G55) I was a making a 5" tall part, and my third vise (G56) I was making a 2.5" tall part, then my fixture height offsets would be:
G54: Z=2.0"
G55: Z=4.0"
G56: Z=1.5"

Each tool being used only has one height offset.
T1 H1
T2 H2
and so on...
 
You can set all your tools to the 4" off the table location and then input the difference of that location from your zero location of each part to each fixture offset. I would either touch off a 1/4" pin on the back of the vise, the top of the tailstock, or the table so when I needed to touch off a new tool all I had to worry about was thermal growth, it was a Fadal after all. I never had a problem with either positive or negative offset values.
 
I am new to the Fadal CNC mill. I am use to Mazaks.

My question for anyone & everyone is can I teach all my tools 4.000 off the machine table and use the G54,G55,G56 for my program "Z"? I want to standardize my 21 tools for all jobs and just teach a "taught tool" off the top of a part for my program "Z". Do I still use a G90 or do I use a G92 in my program?

I really could use the help. I am new here and the only machinist............

I use the shortest tool holder I have as a reference.

Using a conveniant point on a vise or table, I jog down and use a 1.000 gage block to set Z0 (G92Z0)

Then put in a tool and bring it down and find the height of the tool above the table/vise using the 1.000 gage block. If it's say 2.356", I then go into offsets and for length offset I enter 2.356. This becomes the tool off set.

Then I repeat for each tool in the carousel.

So for instance if you have a plate in a Vise, and it's programmed so the top is Z0, then using the reference tool holder I set the height of the refernce tool using the 1.000 gage block, and enter G92Z1.0 as my Z height. Once you've done this you don't have to set the length of the other tools as it's already done.

Most people set their tool lengths using the Fadal utility, I do it my as I prefer to have positive values for tool length as it's easier for me visualise. I can set 21 tools in 10-15mins.

There's a few youtube videos showing setting tool offsets using the Fadal utility

That's how I do it ymmv
 
The way I have found for getting running quickly on a Fadal is to ignore the Z value offsets in the work coordinate systems (G54, G55, E0, E1, etc..) and only set X and Y offsets in your WCS. Let Z remain at zero within all the WCS.

I set tools similar, with a block off the table, so after each is loaded it will be modified to account for the block height (typically done all at once with Mass Modify, after loading all tools). With this, Z zero is the table surface.

Next.. just use the Mass Modify function for all tool length offsets at each setup, based on the desired Z height from the table.

One handy trick to remember what the last 'mass Z' offset, is to offset one additional tool beyond what you have loaded. For example, I have a 21 tool changer, with 21 loaded, but I always do the Mass Modify through tool 22. For the next setup, I first mass modify all tools by the inverse of the tool 22 offset to get me back to zero Z offset.

This method certainly has its limitations, but works great for me when only doing one setup at a time. It keeps its simple, which I find is a good place to start. Good luck!

That's actually pretty slick.
 
I just can't figure out how to teach the program "Z". If I touch the top of a finished part there is no "set" So I look at the absolute Z value and put that in my G54 Then will out moving the tool the absolute Z now reads Zero, so far so good but then wen I try to run the part it will rapid to the top of the part and still have like 9 more inches to rapid? What the heck???
 
You're saying "teach" when you mean "touch". That's confusing people.
.
.
mazak calls it teach with a button labeled teach
.
there is a setting for when spindle face would touch table from zero return position. when you use 4" gage block and tool tip and tell it your 4.0000 off table it is just doing the math to calculate tool length, it knows distance spindle face at zero return to top of table.
.
i would avoid G92 if you make parts where table surface must be zero as part top in vise can change with part changing. i would use G55 to set or compensate for top of part from zero return position and you could set with a tool or test bar if length comp is active to compensate for tool length. or use indicator zero at table top and zero cnc position display and bring indicator to top of part with indicator reading zero top of part and look at position display it will show difference in height
.
some machines there is a button when you press X Y Z all become zero like a G92 X0. Y0. Z0. and you would need to zero return or home the machine to undo if cnc doesnt have a G92 undo command
 
Congratulations "Turbdo1G" you got it right!

That was the right solution to my problem. There is no button for calculating the program Z" like you said it's the difference between the "taught tool" and the top of the part. I put that value in for my G54 Z and it works.

THANK YOU, THANK YOU, THANK YOU,
 








 
Back
Top