haas vf5 tool lengh offset

[crazy^millman]

Well what he is talking about is the ability to hit the feed hold. Then you put the machine in handle and move the head up and out of the way. You have 6 places where you can move it to. You can then change your inserts hit the green button and it will track back through those 6 points at a lower rapid rate through the first 5 then a very very safe feed rate to the last. I would come up like .2 then teach that point then move my great distance at my next point and go from there made qucik work of running through part where you know inserts are going to fail on you half way through the part. So in other words no restart keep running what you were no possible crash becuase it dropped a line of code boom bang done!!!

 

HTH

[Gary]

I have a set up block off in the corner and a touch probe in one tool pocket. I use g59 as the offset to the center of my block. You mdi in g59 x0y0 and touch your probe it will give you an offset number right it down. now you can cal all your tools off this block. Then when you use the probe to touch off your part say in g54 offset All you have to do is enter the number you had wrote down from the g59 probe offset hit f1 to enter the number as its typed now look down at the bottom of the screen and you will see the current height your probe or tool is at type that number in and hit write/enter button. The machine will do your math for you and it won't matter with the +or-. Very fast and accurate. Tools are even touched on the same part of the table each time this way. And if your cutting say a part liine on mold you may not have a float spot left to touch the new tools to if you go off your part each time. hth

[Gary]

I forgot to add I use a 1 in touch pad on the set-block and part, if you take this off the number you write down the first time you won't have to even worry about subtracting it when you touch off on your jobs from then on out.

[cblythe3d]

Caution: The Renishaw probe VQC (visual quick code) uses tool lengths (plus value)balanced by large g54,g55 etc minus Z values. While it works quite well it is not compatible with the native Z minus offsets entered by the Tool Offset Measure button.

 

Haas has included for many years G codes for probing that are straight forward and easy to use. With a minimum effort by using the Haas G codes and macros you can configure the results you desire that are mutually compatable.

 

Charles

[heavychevy2155]

I use to make a clean up cut on the top of the part, and set the tool lengths from that surface. It works great and it keeps from having any numbers in your z fixture offset page, which keeps the confusion to a minimum z zero is the top of the part. But now i work where we use a tool heigth guage, it gets confusing at times. You touch off the tool using the guage, then you do a cleanup on the part then subtract the tool length from the machine position and that value goes in the Z fixture offset. It works if you use the same tools for multiple jobs, but if you change tools often then i would just use the top of the part to touch off my tools, Z0. top of part no muss no fuss.

[ChrisH]

quote:

---

Not sure what "live spindle" means...what does he mean by "crash", software or hardware?

---

The software and the mill, it would skip a line and crash. Haas load a patch but it still crashed ( now this is what the machinist tells me )

 

Live spindle is when you can move X Y or Z with the hand wheel while the mill is cutting. It’s so you can blend to old surfaces.

[DC Gorn]

Just put in a Pre-setter and tell them no more touching off!

 

I just finished a justification for a Pre-setter that remembers all the tools and output a program that will set all the lenth and diameter. All the setup guys has to do is install the tools in the right pocket and run the program. Find G54 and go.

Well some ajustments on those tight tolerances but good to go on everything else.

[ChrisH]

quote:

---

Just put in a Pre-setter and tell them no more touching off!

---

Is it from Haas or a aftermaket pre-setter?

 

[ 08-08-2005, 01:12 PM: Message edited by: ChrisH ]

[MACHINEMASTERG]

+1 on the pre setter we switched to this method and id never go back !!!

[ChrisH]

You lost me for a few I was thinking a tool setter on the mill not a pre-setter (off line)

 

I had a tool setter on my Mazak and Toshiba and there is nothing better then having the mill do the work for you. (The way it should be)

Well the Toshiba had 3 heads (nutating 5 axis / vertical /horizontal) and would not be much fun without a built in tool setter

[DC Gorn]

When you set you tools you are telling the controller how far the tool is from the gage point of you 40 taper pocket. A Pre-setter had a precision 40/50 taper pocket with a known gage height it has indicators with relationship to the gage height. Basicly you put the tool in Pre-setter and it tells you the Lengh and dia. Here is a basic unit.

http://www.commandtool.com/ctstore/showdet..._ID=81&CATID=16

 

Advanced units use a vision system instead of touch indicators.

 

And this works fine with Haas last place I worked used set Z the same way your shop does. After we started using the pre-setter they started bugging be for another one because it was to far to walk to the one we had. We had 12 Haas mills when I left. The oldest was 2 years old.

[MattW]

Hey, I might actually be able to make a contribution to this thread....

 

On a Haas, set setting 33 (coordinate system) to "HAAS". This works just like Fanuc, but doesn't reset g52 when the program resets. I put the length of my offset gauge in my G52 Z value (-2.000 for the electronic guage), so now all tools are set to zero at the point I touch off (top of the vise, most times, in my case). I then put a z value in the g54, g55, etc to offset to where I want z zero to be on the part. This also works pretty good for operations where you are worried about running into the vise- just check the operation of concern to make sure the z value is less than the g54... value. I do my calculations on a spreadsheet- you get a better chance to verify that the numbers you are entering are correct.

 

MattW

Vertex Pharmaceuticals

[MACHINEMASTERG]

Tecknics the tool holder company has an economical presetter (cheap around $$$1500.) that has a 40 taper pocket and an fowler hight gage its what we use on the shop floor on a rolling cart just does the tool lenth from the gage line in the taper we keep a whole bunch of standard tooling all set and taged with there lenth and dia its the only way to go no more tearin down tools and touching of parts for every tool !!!ill never go back now that i have seen the light ...G

[ChrisH]

That sounds great I'm giving a demo today to my Forman on the time savings using a presetter.

 

I'm really thankful for all the input this forum is great!

[PGW Steve]

I forgot how to do all this, I've been spoiled with Renishaw TS27R tool probe and OMP40 touch probe on my 2 VF2's and VF4.

[Jeff2005]

yes steve I am spoiled too I have a TS27R also and when it sets the tool it is set, unless I take it out of the chuck and then I just do a tool setting in my quick codes and it is set again I don't enter nothing takes all of about 1 minute and then I am ready to go again. But, on the other hand I would like to know how to set it like these guys are doing because it may break and then I would be lost.