[CNCCUB]

Just getting started with Haas, manual machinist tool maker for 15+ years, worked with prototrak 2 and 3 axis. Very diferent animals but similar principles. My question concerns tool length offset. I see videos showing touching off the top of vise behind solid jaw using 123 block, then adding -3.000 to number. Then I see videos touching off part itself and setting zero there. It just is not clear to me the touching off the vise or table, looking for a good explanation. Do you do the first prior to your part in the chuck, then do it?

[WOTDesigns]

It depends where you program your datum.

I usually program my datum from the part bottom so I started by putting a 123 on the parallels and ref off that the subtract 3". Then I discovered the edge industries 4" touch off tool and started using that which made it easier to set tool lengths and touch off.

Then I discovered the glorious Haimer 3D Taster probe. Won't live without it now! I have the WIPS probe on my new (first) Haas and wish I could easily use both. The WIPS is great for programing the machine to find center on a part I eyeball in the vise but for set up I'm much much faster with the Haimer. Trade off. Now that I have the wireless tool setter... I'll never be without one! That IS an ungodly time saver.

Brian
WOT Designs

[CNCCUB]

I would want he datum off of the top of the part. So if I did do top of the vise or table originally, I would have to touch again off the top of the part if that was the route I desired or just put the tool in and touch off the top of the part originally? I understand why the offsets are there, no way the programmer can predict what length each tool will be and if you need the length changed, easier to change the length rather than change the program. Still not 100% on this but thank you for the reply.

[Machineit]

I am sure this will quickly veer off to crazy places, but if I were you just starting out, I would keep it very simple.

Set up you part up in the vise or however you need, then touch your tools of of the top of the part. All tools will clear during rapids etc. all programming will have negative Z values. Most every Cad-Cam system writes programs normally in that mode. Z zero is the top of the part and all cutting Z moves are negative.

Have fun-------Mike

[CNCCUB]

Mike thanks for the reply. Keeping it simple to begin with is what I want. I think I understand that if I use a gage block or 1 2 3 block and zero off the top of the vise with all tools they will clear everything good when maneuvering around. i would expect to have a work offset Z option after that where I can set all tools again, one tool as a reference and all adjust automatically, or me measure the difference between where I touched off the vise, table, and add or subtract that amount to all. I see on my screen where I can set tool length offset but on work offset Z remains zero, I can set x and y. So that is not clear to me. When i set tool length offset to the top of the part I feel i can run the program that way just feel there should be a better way. i will be hand entering simple programs.

[Geof]

There is no "better way" just different ways. If you did a search here on cnczone you would find this topic has been discussed at length and sometimes at heat. Just leaving the Z work offset at zero and directly touching off the tools to the top of the part is fine; I did that for years. Eventually I did change to a different procedure when it became tedious touching off several tools on a dozen different parts in a few hours doing small one-offs.

Now I have a reference point that is about 9 inches above the machine table, a height that is above the tallest part I ever do; I touch off onto this so all the tools have a tool offset to this point. This does require a negative value in the Z work offset equal to the Z distance between the reference point and the Z zero plane on the part. The easiest way to determine this is to simply run one tool down to touch the part and take the difference between that tool's offset and the Z position when it is touching. The advantage I see in doing it this way is two fold: First, because the Z work offset is a negative, if you fumble finger and enter a positive value the tool simply goes too high which causes no problem. If the reference point is below the work the Z work offset has to be positive and this time if you fumble finger and enter a negative the tool goes too low maybe with disastrous results. The second advantage is that because my reference point is quite high if I day dream and put the actual Z position in the tool offset when the machine combines this with the Z work offset it will almost certainly exceed the Z travel limit and give an alarm when I check things in Graphics mode.

Now I am sure many people will come along touting the value of probing and saying I am old fashioned, which I am. But I don't have probing, I don't have room for it on my machine table and I can enter ten tool offsets my way as quickly as it is possible to probe them.

[CNCCUB]

Geof

Thanks, I am not looking for the best way, just wanting to get a better understanding. I like the way you explained this. just to make sure, with your zero point 9 inches above the table, once you touch off and and find the difference on one tool, do you change the other tools offset by that amount?

[Geof]

........and find the difference on one tool, do you change the other tools offset by that amount?

No, no; my explanation was obviously inadequate.

All the TOOL OFFSETS are taken to the reference point; in my case about 9 inches above the table but it could be placed at any height within the Z range of the machine.

The top of the part is going to be lower, i.e. closer to the table than the reference point and you want to know this distance; the easy way to measure this distance is to use one of the tools.

For instance take tool 1 and bring it down to the top of the part in exactly the same way as you would if you were touching off on the part. Once there record the Z value in the Position Display showing machine coordinates on a scrap of paper; DO NOT push any keys. Now take the difference between this value and the Tool Offset value for tool 1 and enter it into the Z column on the Work Offset page.

Here is a thread I started some time ago about entering tool offsets. It might be worth your while to read it.
http://www.cnczone.com/forums/haas-m...sets-mill.html

Say the Tool Offset for tool 1 is -2.45 in the Tool Offset page and the Z distance recorded for the Z position with tool 1 at the top of the part is Z-5.73; the difference is -3.28 and this is the value that goes into the Z Work Offset.

When you change to a different part and will be using the same tools all that is necessary is to redo this procedure for the new part; find the Z position for tool 1 when it is touched to the new part, calculate the difference and put this in the Z Work Offset. The Tool Offsets remain the same unless you change a tool at which time you have to touch the new tool off to the reference point.

[Machineit]

No, no; my explanation was obviously inadequate.

All the TOOL OFFSETS are taken to the reference point; in my case about 9 inches above the table but it could be placed at any height within the Z range of the machine.

The top of the part is going to be lower, i.e. closer to the table than the reference point and you want to know this distance; the easy way to measure this distance is to use one of the tools.

For instance take tool 1 and bring it down to the top of the part in exactly the same way as you would if you were touching off on the part. Once there record the Z value in the Position Display showing machine coordinates on a scrap of paper; DO NOT push any keys. Now take the difference between this value and the Tool Offset value for tool 1 and enter it into the Z column on the Work Offset page.

Say the Tool Offset for tool 1 is -2.45 in the Tool Offset page and the Z distance recorded for the Z position with tool 1 at the top of the part is Z-5.73; the difference is -3.28 and this is the value that goes into the Z Work Offset.

When you change to a different part and will be using the same tools all that is necessary is to redo this procedure for the new part; find the Z position for tool 1 when it is touched to the new part, calculate the difference and put this in the Z Work Offset. The Tool Offsets remain the same unless you change a tool at which time you have to touch the new tool off to the reference point.

:drowning:

[Ydna]

If using Geof's method, be sure your setting 64 "tool offset measure uses work" is disabled. If it's on then your offsets get compounded and it's easy to cause a crash unless you happen to notice the odd numbers at a glance.
Verifying your offsets is important no matter what. Use the MDI screen to manually drive a tool to a safe location in order to check your numbers. (be slow and cautious when doing this!)

I agree that setting each individual tool to the workpiece being cut is the more simple method, and likely quicker to set up (especially for simple jobs). Easier to learn that way first, but you might find yourself running into "there has to be a better way" issues if you break a tool and need to re-touch, or if you have multiple workpieces in the machine at once...which is where Geofs concept becomes preferable. It's a little extra work so it can be more difficult to comprehend at first, tho.

[Geof]

If using Geof's method, be sure your setting 64 "tool offset measure uses work" is disabled. If it's on then your offsets get compounded and it's easy to cause a crash unless you happen to notice the odd numbers at a glance.
Verifying your offsets is important no matter what. Use the MDI screen to manually drive a tool to a safe location in order to check your numbers. (be slow and cautious when doing this!).........

I am guilty of not mentioning these cautionary notes but at the same time I advise having Setting 64 on. When it is on, as the Manual explains, the value automatically entered by the Tool Ofst Msr key is relative to the currently selected work coordinate Z offset; i.e., if the Z work offset entry is -2.0000 and the Z position at the reference point is Z-3.000 the value automatically entered for the tool offset is -1.0000 which actually means the tool goes too high not too low. If the reference point was at the table surface, however, I think you could get some undesirable things happening.

The most likely time when the Z work offset entry is relevant while entering tool offsets is if you break a tool and want to enter the tool offset for the new one. In this case because there is a value in the Z work offset instead of using the automatic entry simply type in the Z machine position and use F1 to enter it.

[Ydna]

Do you have a specific use or situation where you use the compounded offsets? Well I should be more specific, I mean outside of the number "safeguard" that you mentioned.

In the college courses, we can't warn people about that enough. We have one old VF1 and one old HL2, where the control doesn't have setting 94 so the mill TLO and lathe geometries are always compounded. it gets worse because the VF1's work offsets are inverted, and again there isn't a setting to flip it to a normal cartesian orientation. it creates a huge demand for running verification codes in MDI, but people still menage to crash things as a result. yeesh
I try to beat it into their heads that any work offset values must be entered after the TLO/geometry to help avoid this confusion, but not everybody follows directions (lol)

I know your enclosures are chalk full with rotaries and vises so I assume that's why you use a riser

[Geof]

Chock full is an understatement. On my personal machine I use for prototyping both parts and fixturing systems I have to use extra short holders or sometimes put in an X, Y move before a tool change so that tools in the carousel rotate past a low point on the fixture.

Regarding offsets I use the direct tool offset, taken to my elevated reference point, combined with the Z work offset to get to the Z zero plane that is furthest away from the center of rotation of the fixture. Then I use G52 to move down the additional Z distance needed when the fixture is indexed to work on the side or bottom of the parts. It gets a bit hairy setting things up for the first time with a new fixture and a new program. Especially when the fixture is indexed 180 degrees and the part is completely out of sight at the back of the fixture.

Once everything is sorted out and the program is proved things are really quite simple. Enter tool offsets to the reference point and run the program, work offsets are read in from G10 commands and any shifts in offsets are done with G52. We can do it this way because we make the same parts over and over again; the hours spent building the fixtures sorting things out up front are recouped many fold when the programs are used.

[Ken_Shea]

I've always used the top of part to set tool lengths, just have never been able to wrap my thinking about the above mentioned method, after reading it yet again I think I am going to kill myself.

[sirgreggins]

Let's say tool 1 is a 1/2" end mill and tool 2 is a .250" drill. Since the drill is longer the Z Offset has to be set. I put a .001" feeler gauge on the top of the part. Then I jog the head down and touch the feeler gauge with tool 1 and press Z, ABS/Set to zero it out. Then load tool 2 and go to the jog function and touch this to the top of the part. Once that touches the feeler gauge, I can go back to the tool table and under the the Z offset column I press ABS/Set. This automatically calculates the difference and sets the Z zero point for that tool.

Do I have this correct?

[Machineit]

This is a two year old post but, you go into jog mode and the touch off of the top of the part with your tool, then you go to the offset page and hit the "tool offset measure" button. Do not go back to jog, just push the "next tool" button, which is right next to the "tool offset measure" button. The machine will change to the next tool and still be in jog mode and will be in .010" increment mode. Touch off on your next tool and hit "tool offset measure" again. Repeat this for all tools.

I would suggest you not touch off tools with a feeler gauge because if you go too far you can chip the ends of carbide tools. I use a piece paper, like a post-it-note. They are .004" thick and and you dent the paper if you go to far without out damaging the tool. At the point the paper is touched stop, remove the paper and then go .003' or .004" down and you are there.

Good luck---Mike

[Ken_Shea]

+1 for Mikes method, obviously not the only method but the exact same one I've used for many years with out a hitch.