Newb question about edge finder z height

[l u k e]

I have a Haimer 3D taster do I set the z height and input into the control as I would any other tool?

[Donkey Hotey]

Why would you need a Z-height for a 3D taster? What method do you use for the Z-height of the rest of your tools?

I think there are a number of strategies people on here like to use. I personally have Renishaw probing on everything I use so, tool lengths and work surfaces are taken care of.

Are you trying to do something similar with the 3D taster and maybe a 2" presetter block? I could see using a tool presetter on the table to set all of your tool lengths. From there, you could use the 3D taster to find the top of the block (indicated by "0" on the taster) then probe whatever your new surface is until it zeroes again. Use the meausred difference as your G54 Z offset and Bob's your uncle.

[l u k e]

I'm asking because I dont know.

I plan on use a 1-2-3 block initially to set my tool height. So by your response I take it it's not necessary, I guess now that you say so its makes sense not to. Sorry for the stupid question, I really didn’t think it through.

[-Chris-]

We Run two Haas VF-4's and set all our tool lengths to a 123 block. on the 2 " side laying on the table. because you can usually find a bare spot to use if you need to change one out. Fixture offsets are set also with a 123 block.

[lkenney]

I use a Blue magnetic Block Gage that has a dial indicator built in it.

I set all my tool lengths that gage set on the back jaw of a Kurt vise, (assuming that I am using vises to hold with). I then barely touch off on the work on a surface that I will machine away, with an end mill.

I hit the reset button to stop the spindle and without moving anything go into the tool setting page. I subtract the current position (bottom of the screen location) from the stored height of the tool from the Blue block. (if the current position is lower than the 2" block height). This gives me a negative Z reading to put in my G54-G129 location zero.

If it is higher you will subract the gaged height from the location height and have a positive number. All tools are then correctly set for that setup. If you break or dull a tool, replace it and zero on the blue block You are redy to go.

Running multible setups? Just run a location zero for each setup (G54 G55) and adjust the Z height settings.

[l u k e]

Where did you purchase the "Blue magnetic Block Gage"? I've looked into many diffrent Z setters and have not settled on one I want.

[l u k e]

I’m a little confused on where the height of the gauge block (or whatever type z setter tool is being used) from the top of the table comes into play. It seems that without that information the control can not figure out where the tool tip or part top is during the z touch of sequence. I’ve tried to find the information in the manual but can’t find anything on the subject. What am I missing here?

I took the Haas class with my HFO and they spent about 30 minutes going over the control and 4 days teaching G code.

[lkenney]

Z-Axis Setter for Mill/Milling-New - eBay (item 230579400926 end time Feb-27-11 13:45:41 PST)

Here is the Z offset gage that I use or one very close to this. I bought mine off e-bay because I have to travel 60 miles to a tool store.

YouTube - Z Axis DIal Tool Setting Gauge
Here is a Youtube with a 50 MM block Inch blocks work the same way.

Lowell

[-Chris-]

I do all the steps ikenny does only i do it all with just a 123 block and i have a brown & sharp gage block .25 thick i set the tool lengths by manually cranking down in MDI to just below the top of the 2.00 height of 123 block then cranking up in .001 increments till 2.00 just slides under tool.go to tool page and push the set length button for the tool in the spindle load all tools and set all heights. Now for offsets i'll set and tram the vice set a stop put a 123 block on the parallels up aginst the stop use an edge finder find x & y.Now i'll load a tool ,one that i set the height on they all have been set @ 2.00 above table so it doesent really matter wich one but i use a tool that is doing blind pockets or somthing and i use the same tool for all fixture offsets.Anyway i jog down till my .250 gage block just slides under tool as i raise it up a thou at a time as soon as it does i go to the tool page and subtract the current height (bottom left of screen) from the length value for the tool im useing to set all this with. now i work from the top of the parallels myself so i would subtract 1.25 from that number and add my stock height all by useing the write enter button to do the math.
Well it works for me any way -Chris

[l u k e]

Originally Posted by -Chris- I do all the steps ikenny does only i do it all with just a 123 block and i have a brown & sharp gage block .25 thick i set the tool lengths by manually cranking down in MDI to just below the top of the 2.00 height of 123 block then cranking up in .001 increments till 2.00 just slides under tool.go to tool page and push the set length button for the tool in the spindle load all tools and set all heights. Now for offsets i'll set and tram the vice set a stop put a 123 block on the parallels up aginst the stop use an edge finder find x & y.Now i'll load a tool ,one that i set the height on they all have been set @ 2.00 above table so it doesent really matter wich one but i use a tool that is doing blind pockets or somthing and i use the same tool for all fixture offsets.Anyway i jog down till my .250 gage block just slides under tool as i raise it up a thou at a time as soon as it does i go to the tool page and subtract the current height (bottom left of screen) from the length value for the tool im useing to set all this with. now i work from the top of the parallels myself so i would subtract 1.25 from that number and add my stock height all by useing the write enter button to do the math. Well it works for me any way -Chris

So the control does not need to know the height of you gage block measured from the top of the table?

[lkenney]

(So the control does not need to know the height of you gage block measured from the top of the table? )

No, it just need to know the difference which I set with the Z zero in the location settings.

Why don't just change the z setting on your location Zero

Like I said above, I set all the tools with the gage block, the sliding of a gage block works but takes time and is suject to feel. The Blue block puts me in at about 0.0004" which for most our work is close enough.

I then take an end mill, usually the 1/2 four flute that lives at station 6 and moving over the material setup to be cut find a point that will be milled away ( I just like as few marks showing when I am done a possible).

I set the MDI for about S1500 M03 hit start and lower the end mill to just off the surface. I then change to 0.001" and gently touch the end mill to the top of the material just scratching the surface.

I hit reset and stop the machine , go to OFFSET and page up the the first tool page where I find my #6 tool

Let's say that I had set a zero for tool 6 off the gage block at 11.567 and that is what is showing in the length setting for that tool. At the bottom of my screen is a line where the current position of the tool is displayed. Let's say that it is reading 12.369

I keep a large button solar calculator attached to the front of my Haas with Velcro. I fire that up and subtract 11.567 from 12.369 which equals 0.802. I am not changing the stored length of tool 6 or any other tool, I am just using the data for caclulations.

Since I am subtracting the orginal tool setting from the current location I know this will be a negative number. If the current setting is smaller than the Tool lengt then reverse the sutraction and the resulting number will be a positive number.

I push the page up buttom which will display the location zero page and let say that I have alread found my X and Y Zeros for G54. I will highlight the G54 Z column and key in -0.802 and press the F1 key which stores it as written in the G54 Z column.

Now all my tools are set to work ib that part with G54 being the location code like this.
G54 X-4.563 Y-3.234 Z-0.802

Now let's say I have a second vise and the part is located at G56 with x & Y at: X-14.567 Y-3.876

I repeat the touch off steps with tool 6 (or any tool that I choose) and find that my Change for the Z height is -1.368. My location for G56 is now
X-14.567 Y -3.234 Z-1.368. I can setup as many offsets as needed without recalculating my tool lengths.

Now all my tools are also set for G56 and I can move between the two vises without any measuring. I often will use the M98 P2345 tocontinue an operation in the second or ther vises havine program 2345 return to O2344 with an M99 before the M30

Just one thing more ------NEVER PUT A TOOL IN THE tOOL cHANGER WITH OUT SETTING THE LENGTH ---- NEVER NEVER NEVER!!!!!!!!!!!!!!!!!!!!!!

Lowell

[-Chris-]

Nope you can use any side of a 123 block any side of a 246 block as long as you use the same for all fixture offsets for that job and do the g54, g55 z settings correctly. essentally When you set the tool lengths all at one spot on the machine you are giving it the difference in length from the tip of the tool to the nose of the spindle its all the same allways as long as you touch them off at the same spot doesent matter whare or with what. and as i allways leave a little stock for first cut and measure things dial in exactly very without much problem. I guess i dont know why people go to all the expense for tool setters and such unless they run a standard tool carousel. then ya but we change out tools for every job and and do moderate run numbers 50 parts or so at a time Chris