[eksinger]

Ok, just when i thought i had this machine figured out. I have a 1990 Vf1
"for a little while now".

I'm trying to set the tools on this machine from a standard location, so
I set all the tools on a two inch side of a 123 block on top of the vise. (negetive value from the reference point) using the set tools button.

Then I'll set part 0 on top of the part by touching a tool to the part, pushing the part zero button. this throws a positive number in the i.e. G54 z x.xx.

from the tool i touched off from I then add the negetive tool hight value to the positive g54 z x.xx. this is the z 0.0 point.. This is the number I insert in the g54 x.xx position using the F1 key.

I just finished a job where i had to add another tool, I touched off the tool to the 123 block like the other tools, and it was way off, (this is where my tool setting issues begin) i've now discovered that this tool is off the same ammount as the g54 z x.xx.

why would the tool hight setting be different once the g54 z x.xx value been set, shouldn't the tool settings be independent of the z coordinate setttings, then what happens with g58,56,57 ect.?

[Geof]

There is a Setting #64, called Tool Offset Measure Uses Work Zero. When this is turned ON any value in G54 Z is subtracted from the Z position of the tool when the Tool Offset Msr key is pushed.

Experiment a bit; look at the Z position display at the bottom of the screen and compare it with the value that goes into the length offset when the key is pushed.

[eksinger]

well, unfortunatly the manual show's my settings only to to 63 which covers tool probes.. i'll double check it on the machine tomorrow. Thanks for the quick reply: )

[Machineit]

Can someone explain to me why some are setting tools to a 123 or some such block. I have been doing this for nearly 20 years and see no benefit to doing that unless you have some job you do over and over and then I find it so easy just to touch off of the top of the part!

I mean I can touch off 20 tools in about 3-4 minutes. So why bother?

I would appreciate the education.

Thanks in advance---Mike

[Donkey Hotey]

The same reason I have Renishaw probing and tool presetters on all of my machines: setup time. I keep a standard tool library in the machine at all times with a matching library in Mastercam. It's also the reason I program from the jaws-up.

I can drop a 123 block in the vise, set my work stop, probe the corner of the block, subtract 1" from the Z-height (the height of the block) and I'm ready to go, all the tools know where the part is, etc. On the 25 pocket machine, I keep at least 15 in it right now.

Edit: that probably wasn't clear enough so I'll elaborate. Without a common reference point in the machine (the 123 block), you can't reuse your tool lengths. If you went to the trouble of tuning all your tool heights to get accurate parts, why lose the offsets each time just because the part location changed?

[Smrtman5]

Greg,

It sounds like that method saves a bunch of time. Do you just keep your 15 most used tools on hand or do you keep all your tools preset?

Using the offsets that way would also let you run in different machines without having to re-touch the tools too, wouldnt it?

[stevo1]

Can someone explain to me why some are setting tools to a 123 or some such block. I have been doing this for nearly 20 years and see no benefit to doing that unless you have some job you do over and over and then I find it so easy just to touch off of the top of the part!

Mike,
I do not doubt your expertise or ability to work your way around your equipment but I have a really tuff time believing that you can touch off 20 tools to a face of a part in 3-4minutes. Half of that time has to be in physical tool changes itself. Along with handling the tool down to the surface of the part with a shim or block and using the measure function and then programming the next tool out.

Yes you are correct that this is most beneficial if you are running the same thing over and over or your tools always stay in the machine. 1 lesson I always teach the guys are when a tool goes in the machine it gets touched off, no excuses. The next guy should know if the tool is in the machine it is touched off. I still have them check clearances though.

It sounds like that method saves a bunch of time. Do you just keep your 15 most used tools on hand or do you keep all your tools preset?

Using the offsets that way would also let you run in different machines without having to re-touch the tools too, wouldnt it?

You will not always be able to use them in different machines as it will depend on the gauge line of the spindle. If they vary a bit then your tools will sit higher or lower but to answer your question they will get you really close. I still believe that if you are going to load tools in the machine then it should be touched off 1 time and you never have to do it again. Now if you are always swapping out tools this really doesn’t matter.

Stevo

[Geof]

Can someone explain to me why some are setting tools to a 123 or some such block. .....

TRADITION. My Pappy did it that way so I am going to do it that way.

Actually my Pappy didn't because he was an aircraft electrician but you probably get my point. It is often personal preference and what you are used to and how your machine is equipped.

[Machineit]

Greg,

Thanks for the info. It makes sense when using MasterCam or some such software. For most of my life I had no CadCam software so always programed by hand. Recently picked up CadCam software so may have to try this. It would not be as big an advantage on my standard 20 tool umbrella as on yours because of your ability to make faster random tool changes.

The place I used to work had an old Roberts and it's tools had to be touch off 1" above the part zero, I though it might have been a leftover from that.

And yes, I can touch off the tools in that time!

Thanks guys---Mike

[stevo1]

I agree with Geof that most of it is what you are most comfortable with. My thought process is more in line with setting up product lines and taking as much of the operator error out of the equation. The more tool offsets you have to do the more chance for error. I even setup my equipment so that the tool offsets are a + positive value and are the value of the GL of the tool. This way when someone looks at the offset and sees 12” but a short EM comes out that is about 3.5” in length it throws a flag that something is not right. I do the same with the work coordinate system so that if the part is 5” tall 5” is what it is set to. There has been many threads discussing this.

Mike,
I am impressed. That is 12sec per tool. NASCAR pit crew’s aint got nothing on you

Stevo

[Donkey Hotey]

It sounds like that method saves a bunch of time. Do you just keep your 15 most used tools on hand or do you keep all your tools preset?

We have the Renishaw tool presetter so, the tools are always preset as soon as they go into the machine. This is for a prototyping and short-run environment where setup time for a few parts would kill us and there are already 2-3 potential operators who might need the machine in a week. That meant that there needed to be some standards established. This is what I came up with. I'm certainly no expert on this so if somebody has a better system, I'm all ears.

The idea was to load all the standard cutters that we might need for any given job. That meant an assortment of endmills and face mills. We include an engraver and 1/8" corner rounding tool (if it's in the machine and convenient, we use it more often in our designs to make things more pleasing to handle). We use 1" and 2" inserted shouldering mills as well as a 3" angled facing mill. We include a 100 degree countersink (aircraft fasteners) that also doubles for small chamfers. That covers tools 1-12.

The Renishaw probe is Tool 25 (always the last tool on whatever machine we have). From the probe, I back down the next four pockets with drill chucks. If there is a drill in the machine, it's in one of those pockets (24 down to 21). Rarely does a part have more than two taps so Tool 19 and 20 are reserved for taps.

That leaves six pockets to load odd-ball tools. If the job needs a dovetail mill, it's in one of those. More taps? It's one of those. A different corner rounder? It's one of those.

This table matches what we have in our standard tool library in Mastercam. I can import a solid model into Mastercam, suck in the tool library and get to work programming it. I know that the left vise has step jaws in it. I program G54 as the back of the fixed jaw, bottom of the step and against a work stop or I probe the left edge (as appropriate).

If we had to do some simple feature, we can literally pull in the solid model, have it programmed and cutting chips in 15 minutes: almost zero setup time (except maybe probing a 123 block to establish G54). It works very well for us, though it's always evolving to meet our needs.

1 1/8” Endmill
2 3/16” Endmill
3 1/4" Endmill
4 1/2" Endmill
5 3/4" Endmill
6 1" Endmill Indexable
7 2" Facing / shouldering
8 1/4" Ball
9 100 degree c-sink / chamfer
10 1/8" Radius Corner Rounding
11 Engraving Tool
12 3”, 45 degree Facing mill
13
14
15
16
17
18
19 Tap
20 Tap
21 Drill chuck (general use)
22 Drill chuck (general use)
23 Drill chuck (general use)
24 Drill chuck (general use)
25 Renishaw Probe

[eksinger]

There is a Setting #64, called Tool Offset Measure Uses Work Zero. When this is turned ON any value in G54 Z is subtracted from the Z position of the tool when the Tool Offset Msr key is pushed.

Experiment a bit; look at the Z position display at the bottom of the screen and compare it with the value that goes into the length offset when the key is pushed.

I double check my settings.. the settings only go to 63.. must be an earlier model, the serial number is in the 1400 series.

[Smrtman5]

Greg, Thanks for the info!

[metlshpr]

When using a 123 block to set all tools; the g54 z setting is just a measurement from 123 block to part zero. Its simple: if part zero is under 123 block then value is -, if above than +.

[eksinger]

When using a 123 block to set all tools; the g54 z setting is just a measurement from 123 block to part zero. Its simple: if part zero is under 123 block then value is -, if above than +.

yes, i understand that's the way it should work. and i've had it work that way on most machines. but this one isn't cooperating the same way.
i'll set all the tools to the 123 block, then set the g54 setting. (still having to add the negitive tool offset to the g54 part z zero) but if i have to set another tool ( one the 123 block ) the tool is off by the g54 ammount.

this is an older haas.. it has no setting 64.

guess i'll keep playing with it till i find its preferred personality.

[stevo1]

Could it be that it is taking into account the value in G54 when setting the tools. I don't like using G54 for part data just because on the controls I am use to (Fanuc) G54 is default so it always carries the value when just doing simple positioning or MDI work.

I would use G55-G59.

Stevo

[KenFoulks]

You can erase the work offsets before you set your tools. What software version do you have? I can look up setting 64, see if it used to be something else.

[eksinger]

You can erase the work offsets before you set your tools. What software version do you have? I can look up setting 64, see if it used to be something else.

vresion 3.1 poppes up on the screen when i power up. typically i'll set all the tools first, then i'll set the g54 z axis on top of the part. however something tells me i'm doing it wrong on this machine.. when i push part zero, there is a large positive number in the z display. i'm having to add the negitive the tool height value (from the tool i'm setting with) to this number and key in that value in g54 z line to get the proper setting. also if I add another tool, I will set it off the 123 block. then have to subtract the value of the g54 value from the tool height setting to get the tool set correctly. the manual indicates to set everything off the top of the part. but i'm trying to get the tools to set off a standard setting.

[KenFoulks]

Setting 64 was created to address this issue. The only way around this to keep G54 at Z0 and use it to set tool offsets.

Detail: G54 Z value is to always remain at zero. Have G54 active whenever you are setting a tool offset. You can use setting 56 to help keep G54 active. Another possibility is to clear the Z value before you use it, but this has crash potential.

[stevo1]

Or as I suggested before you can always leave G54 zero so your tools are set properly every time and then use any one of G55-G59 for part height.

Stevo