Fadal Toolsetting method

[Cole2534]

Tool height and library management has always been the hardest part of milling for me. And while Mr. Gough has an excellent tool setting method, it's is a little more advanced than I was wanting to try at first. After explaining my method to someone yesterday I wrote it down and figured I may was well post here for both sharing and critique. It does use a 3D taster, a Haimer for me.

Step 1) Set Haimer to tool #1, and zero it on the reference plane. I chose the table so that all offsets were positive values. Note this value. I wrote it in sharpie on the 4020's door frame, I use it a lot.

Step 2) Set all tools, #2 - #22, to the reference plane. This doesn't necessarily need to be done all at once, just need to be consistent in measuring new tools to the reference plane. We go through #22 so our Z offset is noted in the control.

Step 3) Use Haimer to measure Z offset. This can be done 2 ways.
Step 3a) Locate part Z zero with Haimer, subtract this value from the Haimer's H value to get the Z offset. Don't get lost in the +/- side of it, by going from the table you're taking the number's absolute value.
Step 3b) In MDI, call up T1 and jog to an unused portion of the table. Call H1. Haimer will go to ref plane. Now use jog to find Z zero. This method does the math for you, but opens you to the risk of crashing your probe.

Step 4) Mass modify #2 - #22 with the Z offset.

Step 5) Check yourself before you wreck yourself. Pull up the tool table and ensure that tool #22's value is a reasonable number.

This keeps all your tools at a common Z reference point and is great for use with known fixtures. It also allows you to use the fixture offset Z for small tweaks in an easy to see method. IE- E11 Z-.001 instead of a full number, if that makes any sense.


This is very elementary to most here but maybe someone will need it some day.

 

[vmipacman]

So you have to modify all tools used when going from one work offset to another? Step 4.

sounds like an error trap but thanks for sharing.

 

[Spruewell]

I dedicate G52 for tool setting. Find a reliable datum ( I use the top of my 4th axis) and set its Z0 according to a known length tool. I have a dedicated side-lock with a 1/2” carbide tool shank set at 4” that I use across all my (2) machines. I don’t actually touch off the datum, but use a 1/2“ round carbide tool blank. When the blank just passes under the 4” reference tool I set G52 to X0 Y0 Z0. All my tools are then ”touched off” at this common point and tool lengths recorded No mass adjustment required. work offsets can then be set similarly with any tool. You must however adjust the work Z offset by the length of the tool used to “probe” it. This method allows me to swap tools between machines and transfer their tool lengths. A tool with a 3.1234” tool length in one machine will have the exact same 3.1234” tool length in the other machine

 

[lobust]

If you already have a Haimer the very best thing you can buy to accompany it is one of these (picture below).

I have 3 or 4 of those on the shop floor, along with some fancier Nikken ones that I use on the mills usually, but they are way more expensive and not necessarily better.

On the Fanucs I dedicate G58 to tool setting, although on smaller machines you can just use any work offset that is zeroed. I use G58 because zeroed doesn't work on larger machines as Fanucs can't accept a tool offset larger than 999.999mm. I digress.

Set the haimer on the reference edge and tools on the plunger. Then use the Haimer to set the work offset on the part. If you have a work offset dedicated to setting tools, just call it up whenever and set tools without affecting anything else.

 

[Cole2534]

So you have to modify all tools used when going from one work offset to another? Step 4.

sounds like an error trap but thanks for sharing.

You don't HAVE to modify them all, but in doing so you keep them all the same. On the 88HS controller if you're going to modify one offset its only one additional keystroke to modify them all via the 'Mass Modify' command.

 

[Cole2534]

If you already have a Haimer the very best thing you can buy to accompany it is one of these (picture below).

Got one. It's a huge time saver.

 

[Mhajicek]

Am I understanding you right? Are you changing each tool length offset when you change your work Z? Why not use work offset Z?

 

[Mud]

Is this really less work than measuring the tools on a surface plate and inputting the numbers? I've never done any Fadal.

 

[Spruewell]

Most machines have a “tool length offset” button which greatly reduces the chances of fat fingering a tool length that was measured outside of the machine. ”oops! That was supposed to be 5.34” not 3.54”….”

 

[Herding Cats]

It's also not super involved to write a macro that populates the value for you. If you have G31 skip you could also set up a semi-auto too setter.

I highly advise against using tool height offsets in place of Z fixture offsets. IMO tool height offsets should only be used to reconcile the difference from gauge length, spindle face or a master tool or probe.

If your control will use negative tool offsets them you can set the probe as zero and all tools in relation to that. Then when the probe is in the machine the machine coordinates will be the actual values to enter in a fixture offset with no math.

My OKK with a Haimer is set up this way and has a switch with a value you populate from home to a reference surface so when you press input it populates the tool height offset value. This number is the machine Z coordinates when the Haimer is touching the tool reference surface. Again the Haimer has no Z offset.

My other machines have probes and tool setters and are not configured to auto populate negative tool offsets so I run then as designed off of gauge line.

Hope this helps.

 

[lobust]

It's also not super involved to write a macro that populates the value for you. If you have G31 skip you could also set up a semi-auto too setter.

I highly advise against using tool height offsets in place of Z fixture offsets. IMO tool height offsets should only be used to reconcile the difference from gauge length, spindle face or a master tool or probe.

If your control will use negative tool offsets them you can set the probe as zero and all tools in relation to that. Then when the probe is in the machine the machine coordinates will be the actual values to enter in a fixture offset with no math.

My OKK with a Haimer is set up this way and has a switch with a value you populate from home to a reference surface so when you press input it populates the tool height offset value. This number is the machine Z coordinates when the Haimer is touching the tool reference surface. Again the Haimer has no Z offset.

My other machines have probes and tool setters and are not configured to auto populate negative tool offsets so I run then as designed off of gauge line.

Hope this helps.

There are so many different ways of doing this and all controls handle it a little differently. It seems that most of us don't know anything about Fadals, so we may be just posting irrelevant information anyway.

I have machines that the TLO is the absolute length of the tool from the gauge line, machines where the TLO is the distance from machine zero to the datum gauge on the table, others where the TLO is the distance from a completely arbitrary position to a fixed gauge. Depends on what the control is or isn't capable of.

I really only use a Haimer anymore on one machine, an old Hurco. It has one work offset, no additional fixture offsets. It is not convenient on that machine to use a TLO of zero for the Haimer, as you would then have to measure the Z work offset on the setting gauge before setting the other tools. It's much easier to zero the Z work offset and measure all the tools, Haimer included. Then when you are halfway through a job and need to measure some new tools, you only have to set the Z work offset to zero in order to measure them, rather than an arbitrary number that you'd have to write down somewhere.

Another quirk on the Hurcos (including the newer ones where the tools are all probed) is that there is an additional "Z offset" in the work offset that can be populated if required to shift the z offset up or down for chasing tolerances or whatever you might need it for. Behind the scenes, it actually adds or subtracts that value from all the tool offsets, which sounds very similar to what Cole is talking about on his Fadal...

 

[Cole2534]

Am I understanding you right? Are you changing each tool length offset when you change your work Z? Why not use work offset Z?

Yes, but they're done en masse so it's one adjustment. My Fadal, not sure about others executes Z fixture offset as a move. If that move exceeds allowable travel, in my case is over +4", you get a limit alarm.

It's dumb, I agree. But it still makes me money

 

[Mhajicek]

Yes, but they're done en masse so it's one adjustment. My Fadal, not sure about others executes Z fixture offset as a move. If that move exceeds allowable travel, in my case is over +4", you get a limit alarm.

It's dumb, I agree. But it still makes me money

A long time ago I worked for a guy with a '90's Fadal. He set tools normally, relative to the table, and used Z in the work fixture offset. That way you can have multiple fixtures setup at the same time, at different heights, and use the same tools across all of them.

 

[Cole2534]

A long time ago I worked for a guy with a '90's Fadal. He set tools normally, relative to the table, and used Z in the work fixture offset. That way you can have multiple fixtures setup at the same time, at different heights, and use the same tools across all of them.

I'd LOVE to do it that way, but so far I've only broken tools trying it.

 

[atex57]

I'd LOVE to do it that way, but so far I've only broken tools trying it.

Easy peasy to coin a phrase. Set all your tools relative to the table and set your work height with your fixture offset (Exx). Effectively height of workpiece Z zero from table. I can write up a complete description if you like.

Ed.

 

[Cole2534]

Easy peasy to coin a phrase. Set all your tools relative to the table and set your work height with your fixture offset (Exx). Effectively height of workpiece Z zero from table. I can write up a complete description if you like.

Ed.

I tried that, it doesn't work for me. I described it somewhat in post #12 in this thread, but I'm on a real keyboard now so will give more detail.

The way the control handles the G54/etc offsets in Z is the same as it does in X/Y. G54 (or E1 specifically) is called, it moves to the offset position from home and the new position is 0,0,0. It treats XYZ as a coordinate shift. If i have a G54 offset of 2.0, 2.0, 2.0 the machine makes a Z move of 2.0", the makes an XY of 2" each way. The limitation I have is that from machine home (cold start position) I only have 4" of positive Z travel (and 16" -Z). So if my G54 Z offset is >4.0" the machine will alarm out on soft limits at 4.0. Given that Kurt vise beds are 2.875" off the table,

If I was designing the control, I'd have made the control so that Z was automatically accounted for in tool length, rather than a coordinate shift.

I'm not explaining it well, probably because I don't understand it well. However, I've not found anyway better in all of my research. If a better mousetrap is out there, so to speak, the inventors are keeping their lips tight.

 

[Herding Cats]

Are you saying if the machine is at 0 0 0 and you just call G54 it will move to G54 0 0 0? If so on a Fanuc that is a parameter change and I wouldn't be shocked if Fadal also has a way of controlling it.

Also your Z values for G54 should always be a negative number. You are reconciling the difference between machine 0 and part 0 which will always be a negative number unless the part zero was above home which sounds impossible to me, although now that I think about it Fadal machines don't home at the end of travels do they.

 

[atex57]

I tried that, it doesn't work for me. I described it somewhat in post #12 in this thread, but I'm on a real keyboard now so will give more detail.

SNIP

I'm not explaining it well, probably because I don't understand it well. However, I've not found anyway better in all of my research. If a better mousetrap is out there, so to speak, the inventors are keeping their lips tight.

First off, how are you doing to put tools in the tool table? How are you setting the tool table?

There are a couple of ways to do that and they are incompatible.

Ed.

 

[Cole2534]

First off, how are you doing to put tools in the tool table? How are you setting the tool table? with the tool-setting routine in the control. Tell control height of block, touch all tools to it, it compensates for block

There are a couple of ways to do that and they are incompatible.

Ed.

Are you saying if the machine is at 0 0 0 and you just call G54 it will move to G54 0 0 0? yes.

although now that I think about it Fadal machines don't home at the end of travels do they. they home in the center of travel in xy, and at tool change position in z.

Answers in bold

 

[atex57]

Answers in bold

When I got a Fadal I started watching YT videos on tool changing and setting.The best lesson I learned was to leave E1 as all zero's. Are you using fixture offsets? If not you need to learn them and setting Z offset in the fixtures. I use E2 X and Y as the corner of a vise and set Z to the height of the top of the part ( Z zero ) from the table. E4 is generally the center of a 3 jaw chuck bolted to the table, then other fixtures get different offsets.

Ed.