I need some help on the procedure of setting the offsets. I have followed the book but comimng up off the part. I need step instructions sense I am missing something. Some help would be appriciated sens I am new to this machine.

What machine is it ?

Is this a mill or lathe are you refering to the tool length offsets?

VF3 vertical mill

Assuming your talking about tool length offsets, for just drilling & milling holes bring the tool down till it either touches or very close to touching the part, hit the offsets button. If the highlight bar is not on the tool your setting up then arrow up or down to get to it, this is very important the highlight bar needs to be on the numbers part(ex 12.0314) this will be at the left most part of the screen once it is there and you have the tool height where you want it hit the tooloffsetmeasure button. Is that what you wanted to know?

also your z numbers will be in the negitive (in your program you are running) to do any maching on the part

I am setting the tools to a measured block on the table from the carosel. Than what I need to know is how to setup the g54 of the part offsets. I know to use part zero for the x and y but the z of part zero is not working out. I also need to check the program for the negative #. I am using master cam for programing. THis is a simple setup but driving me nuts!

So you have your tools all set to the reference block. Now, with the last tool still touching the reference block, go to your position/operator screen. If the Z axis was the last axis active, it will be flashing on this screen. So press 'Origin' to zero the Z axis display. Now, you can jog over to the part and touch off of it. The Z axis display will now measure the distance you have moved, from the reference height. Enter this value into your Z G54 offset. Observe the sign of the value.

i bet he is not useing G43 h (tool number)

. I am using master cam for programing.

I doubt that G43 is the problem

the way you are setting your tools makes your G54 or G154 Z value an incremental value from your reference block the post in master cam will do what you assign it to do.
your Z move to top of part should read

G90G43Z#H#

Just curious but why enter the work coor Z at all? What I was taught, hand coding and using mastercam was to do the following:
*Set the top of your stock to Z0.0 (default in mastercam parameters)
*After posting the program set up your work, insert your tool(s), touch off on the top of the stock, go to Offset, cursor/page down to the Geometery Length by tool # press the Tool Length Measure button, cursor over to length wear, enter a negitive value matching the mic'ed value of the shim. *Repeat for all tools used in the program.

Why wouldnt this work for your application? As a recent graduate I still am learning the capabilities of the machines I am programming and running but shouldn't this work? If not let me know before I find out the hard way if not ;).
Scott

Scott,
That method will work, if you set all your tools off the same piece, and never have to add or change a tool (with an accurate Z height requirement). However, the accuracy of most 'stock' might be +/- .005" or so and add to that that some stock clamped to the table is in a warped condition. So 'top of stock' is not a repeatable reference height.

I learned of this the 'long way' :D I was cutting a mold one time, and had set all my tools somewhere off the top of the stock. I got into cutting it, and in the course of this, one small endmill plugged up and broke off. So I installed a new tool and touched off the partially completed mold and carried on with machining. Now what I overlooked, was that I had had to increment my Z work offset down a little bit from zero at some point in the program. So the original 'top' was now a little lower than where all the rest of the tools were set.

This oversight cost me several extra hours of machining, because the new tool overcut the finish depth by a few thousandths. So I had to go back and recut the entire finish pass to get it all relatively correct. Once was enough.

Now, I use a reference block with a Z setter as a habit, any time I change or add a tool. Its the habit of using a known reference that is valuable. If you are always cognizant of what the pitfalls of using a floating reference are, you can work around it, but it is likely a comparatively rare event to remember that a new tool has a different setoff height than the rest of the set, so I figure its just a matter of time before you get caught like I did. So maybe you throw a $2 piece of stock in the scrap? Who cares? You will when its a $500 piece of stock :)

An alternate approach to Hu's is to touch off on the raw stock then move down by whatever amount you will be removing and have the finished surface as Z zero. Then if you wipe out a tool you simply touch the replacement tool off on the finished surface.

Just curious but why enter the work coor Z at all? What I was taught, hand coding and using mastercam was to do the following:
*Set the top of your stock to Z0.0 (default in mastercam parameters)
*After posting the program set up your work, insert your tool(s), touch off on the top of the stock, go to Offset, cursor/page down to the Geometery Length by tool # press the Tool Length Measure button, cursor over to length wear, enter a negitive value matching the mic'ed value of the shim. *Repeat for all tools used in the program.

Why wouldnt this work for your application? As a recent graduate I still am learning the capabilities of the machines I am programming and running but shouldn't this work? If not let me know before I find out the hard way if not ;).
Scott


the reason he needs a Z coord is that he is setting his tools from a reference block and not the top of the part. this makes his part zero a Z distance from the top of his reference block to the top of his part. setting tools this way makes your set ups easier where you have programs using the same tools. you do not have to retouch the tools for every set up, all you have yo do is reset your Z coordinate. The way i set my tools all my TLO are positive. the number i have is actually the distance from the nose of the spindle to the tip of the tool. My Z coord is a very Huge negative number which is the distance from the nose of the spindle to the top of the part. the reason for this is we normally have about 3 to 4 jobs in the machines at one given time. all we do is change programs to run what part we want to run, our X Y & Z coords are loaded thru the programs with G10 commands. I hope I made some sense here.

..... The way i set my tools all my TLO are positive. the number i have is actually the distance from the nose of the spindle to the tip of the tool. My Z coord is a very Huge negative number which is the distance from the nose of the spindle to the top of the part...

We do a similar thing on some of our machines with a little difference. Our system uses negative TLO and also a smaller negative Z in the work coordinates. This approach was taken after learning a nasty lesson: If somebody fat fingers what should be a positive entry and instead puts it in negative the tool goes down into hard stuff. If the entry should be negative but somebody puts it in positive by mistake the tool simply hangs around stirring air. Stirring air is less noisy and cheaper.

I appreciate the edification. the biggest draw back to my job is being straight out of school it is assumed you will work in a shop with experianced people surpervising you, teaching you etc. That isn't the case in our shop, until recently I was the sole machine shop employee. Now I have a conventional guy that I'm learning from, plenty of mistakes I'm trying to learn from, however I really appreciate all the explanations and help I've recieved here. It is always nice to learn from someone else's hard lessons ;)
Thanks for the explaination
scott

I am working with a 1995 VF1 WITHOUT a tool presetter.

I have read the pros and cons to setup techniques, and wanted to dive into this topic further.
I have experince with a Haas lathe with a tool presetter. On the lathe, most of the tools remain in the magazine, and therefore, so do their presets. This makes setting up work in a job shop environment where I run at least one new and different job every day, quite easy. All of the tools have been defined by the presetter, so, I load a part in the chuck, touch tool 1 off of the face of the work, and hit the z measur button to transfer that number into G54. Easy.

Now that I have a mill with a tool magazine that holds 20, this seems to be a natural. After reading multiple Haas manals, I am more confused than ever. Setting 64 "tool offset meas uses work. -- off or on??
Today I gave a Haas tech a scenario where I preset all my tools to a gage block. He says that I cannot simply touch a known tool off of a work surface, and press a button like I do on my lathe, that I have to manually enter the difference between my gage block, and my work height, as I have read in a previous post.

I want to get this right the first time, I'd rather not learn a better way later, and have to relearn everything.

Thoughts?

I cannot answer why Haas mill does not have 'one button setting' for the Z work offset, but AFAIK, we would have to have a parameter setting such as most lathes already have to define the tool presetter position (in the machine coordinate system), except in the case of the mill, I guess we would want to predefine an arbitrary plane height (our gauge block height) or perhaps use the table itself. Some guys do, but not always will the tools actually reach the table, so that can be a problem.

FWIW, I use a 2-4-6 block with a 2" high Z setter (dial gauge thing) for my tool setting plane.

Lately, I have evolved the method I described above, using a digital height gauge to measure my Z work offset. I have not actually changed the logic, I would call this a shortcut. What I do now is zero the digital height gauge on top of my 8" gauge stack. Now, I can just place the height gauge on the table, touch off the part, or indeed, firstly examine a piece of stock for flatness to gain an average workable reference on the part, whatever, and the direct reading given on the digital height gauge display is my work offset.

This is barely more convenient than using one of the tools as described above, and the operator display to measure the distance. I started using this method when I had some irregular weldments to set up, and needed to survey the part in a few places before determining what the Z workoffset should be, and all the parts were slightly different.

I actually learned more from reading the posts in this thread than I did in the Haas manual.
We experimented last night, and the idea of using the control as a readout to give me the difference between my "gage" and the work surface works perfectly.
I called my HFO about buying their probe system, but they haven't quoted yet. We're ready to go for the porbe system. We use a touch probe for x/y work setting on two other mills, and it saves montain of time.
the tool presetter on the lathe does the same.

when i'm seeting a tool off in the vise i uae a 1.5 gage block..and i use 1.5 parrells so my z off set is always a positive number.so when i put a new block i just change the z off set..i do the same thing if i'm doing plates i set my tool off a 1" gage block off the top of the blocks i'm clamping the blocks to so all i'll have to do is change z offset

We're using a Renishaw tool setter at work, but I used to operate a MAHO without one. What I did was:
-Put the first tool in a tool holding fixture and zero a height gauge on its tip
-Put each tool in the fixture, measure it and write the length down
-Go to the tool offsets page, set the first tool as 0 and the rest as I measured them
-Touch the first tool off and set my Z (actually my Y cause it was a universal mill)

It was faster and more accurate than touching every tool off. The first tool doesn't have to be T1, it can be anyone. I normally used the biggest endmill, T1 was almost always a spot drill.

Nikolas