Haas VF fixture offset hell

I read through these posts, and thought what the hell I throw in a suggestion or two. I think this is similar to some of the posts but I
didn't quite follow all the techniques
I run a VF0E, usually with two to three vises. I program for this machine with Solidworks and Camworks. The tool crib / library works well with this setup. My prefered method is to touch off Tool 1 to any convienant spot on the vise, table, or part. A good flat surface. I run predominatly aluminum so Tool 1 only gets changed every so often, it could just as easily be the 3-axis probe.
The TLO register for Tool 1 is left or set at 0. In the G54 Z work offset register I record the z value of tool 1 using the Part Zero Set button. Wether I use a gauge block, 1-2-3, or a single axis led probe to touch off, doesn't really matter as long as you are consistent for all tools. Next I load tool 2, touch off to the same location and use the Tool Offset Meas button to record the difference between tool 1 and tool 2, in the tool 2 TLO register. It is possible to do this offline but I don't have the set up to do it. So Tool 3 goes in, touch off to the same location, Tool register records the difference between tool 3 and tool 1. Same for the rest of the tools.
I keep 8 tools loaded in the tool changer and all are set in relation to tool 1. When I change setups I use the edge finder to locate x and y, and the touch tool 1 to the top of the part and record the work offset in the G54 Z register, again with the Part Zero Set button. All the rest of the tools follow it, so they are set. Next I go over to G55 part touch off its z work offset location, then G56, etc. If the vises and stock are consistent you shouldn't see more than a few thousandths between z work offsets. If you are using the 1-2-3 block you obviously have to subtract that distance in the z value. Next if I am running a flycut pass to clean up the top I go back to the work offsets and subtract an additional .010 or so out of each z value, checking that my deepest tool move will still clear the jaws. Minor adjusts for depth in individual tools I use the wear register, just like the diameter compensations.
If I need to add tools to the mix, and have already machined the top surface of G54 which happens to be my Z 0, I touch them off to that suface and record their differences to tool 1. I am still touching off several times with this method but I don't have to do it for every tool, every setup, and additional tools go pretty quick.
I was trained to touch off each tool to the top of the part, and it took a little adjustment to make this transistion. It is getting late here so I hope this makes sense, and helps you out. Regards, JL

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
There are a few different ways to set your work offset in the Z without touching off every tool. (You should never under normal conditions need to retouch off a tool). 1. If there is a value already in your work offset Z: Call up the tool you want to use(any tool should do, provided that it has been set) bring the tool down and touch off of the part. With the tool at that position, go to your tool offset screen. The length offset of the tool you are using should be highlighted. Take that number (without the negative sign) and subtract the Z position number at the bottom of the screen. Go ahead and manually type in the number you get at the bottom of the screen. Hit the offset button to get to your work coordinates screen and cursor over to where you want to set your Z work offset and hit "write/enter" 2. If you are setting a tool and need to set your work offset also: When you touch off your tool, and hit "tool measure" Do not move the tool but go to your operator position screen and zero your Z (using the "origin" key). Then move the tool to where you want to set your Z work offset and touch off tool. The value that is in your position screen (Z) is the value that you enter in your work offset.
You can clear all of your work and tool offsets by going to the screen you want to clear and hitting the "origin" key. The control will ask if want to zero all y/n.
bytecolor wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I use pretty much the same routine to vary our machine Z heights for the "familys" of parts we run. It works in the vertical machines but don't try it in a horizontal. If you use a "safety block" at the start of each tool (g0g90g49z0) or send the machine back up to Z0 in program you are also limited to a Z+ grid offset amount equal or less than the distance from the Z tool change point up to the Z+ over travel point of the axis so don't use the table as Z0 for tool cal. That's why it won't work on a Haas horizontal, they will not travel above the Z home position like the vertical will. If you change fixture heights frequently be sure to use one of the taller ones to set the tools to.

My machine sets any individual tool length offset relative to the machine Z "home" (tool change) position regardless of the grid offset. Look at the "position" page when you set the offset, the offset value should be the same as the Z in "machine". If not there must be something set different than mine was when delivered.
If I have to replace a tool I touch it off on the top of the offending part and set the offset as normal, then add in the OPPOSITE value of the Z offset that's in the grid I'm working with. Say I have a Z+1.000 in the g54 grid used in the program. I touch off the tool and set the offset just like normal then I put in "-1.000" and write. This compensates for the 1 inch higher the tool will be when running the program in the G54 grid. It also keeps all the tools relative to each other whichever grid used.
Hope I didn't confuse more than helped.
JohnF
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ok, Admittedly, I'm not an everyday mill guy (lathe guy mostly), but from my control experience, I am having problems understanding why all the different methods. And maybe I'm wrong on this, as there may be complications I'm not seeing....but here are my thoughts.
If the reference point of the machine is correct, the distance should be known from machine reference to the mill table.
If not, you should be able to use the 123 block method, or set up an indicator on the table and use Jo blocks to Zero it at a known distance, then using the machine coordinates on the control, bring the spindle down to where the indicator reads zero and add the jo block distance.
The control should remove the distance of any TLO from the machine reference distance automatically when that TLO is called. It should remove any distance difference between the Work offset and the machine reference point automatically when the WO is called.
So in effect, you should be able to plug in a G54/55/56, etc and a TLO and it should work out exact.
Now, where the G54/55/56 ect comes from may differ from one control to another. Some may come from the table up, some may come from the spindle down. The sign in your WO and TLO is also important.
So...as an example..
Say the control does show 0,0,0 at reference (I hate that, btw), and the known distance from reference to the table is -580 mm (it would be negative in this instance). Now your distance from the table to the Z0 on the part is say 180 mm, you should be able to plug that into G54 as a POSITIVE 180 mm. When the control does the addition, it comes up with -400 mm as the distance to Z0 from machine reference. Now you have a tool that is 120mm long, and you put that in the TLO as a POSTIIVE 120mm then when the control does the addition, it should come up with -280 mm to the part from the tool tip. The opposite on the signs would need to be used if at reference the machine shows something like 120,100,580.
If things are set up this way, you should be able to use a simple height gauge to measure the work offset from the table, where practical, plug in the value and go.
You could use the indicator method for tool length.
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
So, I finally get back on the Haas and do a bit more fscking around. Thanks to Brents tip on changing setting #64 to OFF, I don't have to worry about what fixture offset is active. The procedure goes:
1... Hit reset, this activates G49 on my Haas, thereby canceling any tool length offset. 2... Touch off any newly installed tool to a fixed height. A 1-2-3 block resting directly on the table in this case. Wheel the tool down, touch the block, using a .001 feeler. Hit TOOL OFSET MESUR. NEXT TOOL. Rinse and repeat for each newly installed tool. Ultimately I'd like to use one of those tool setters like Bob mentioned. 3... Use any tool that has been touched off using step 2 to set part Z zero for each fixture offset. Wheel the tool down to the point where you want to set part Z zero. Top of the stock most times in our shop. Move the cursor to the Z coordinate of G54, or whatever fixture offset you are setting. Hit PART ZERO SET. Now enter the tool length offset of the tool you just touched the stock with into the G54 Z coordinate. This, of course moves the Z incrementally. 4... Repeat step 3 for the other fixture offsets you are using. 5... Done! (with the TLOs and fixture offset Zs anyway)
Works for me.
--
bytecolor


Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.