I set all of my tools 2" above the table. Then when I set my zero for the top of my part. I subtract 2" from that to get my part zero. Is there a parameter I can set so I don't have to subtract from the part? I have a guy who can't get this concept through his head and I would like to take all the math out of it to prevent mistakes. The nice thing about it is if they forget to subtract from the part, they just cut air instead of crashing.Is there a better way?
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Hass tm3p tool setting
- Thread starter rbregn
- Start date
- Replies 5
- Views 1,428
G00 Proto
Hot Rolled
- Joined
- Feb 18, 2013
- Location
- Dirkdirkistan, ID
I set all of my tools 4" above the table (1" block plus a 3" dial height gage). My Z offset on the xyz offset page is the distance from the top of the 4" gage assembly to the top of the part. I never do any math. I just use a dial indicator (or test, or Haimer) and go to zero on the top of a 4" block, hit MDI then Handle Jog. That zeros the DRO. Then I dial in the top of the part. The number on the DRO is the offset that gets put in the Z offset.
It sounds complicated, but it is dead easy and I never mess it up. I also make use if the nice easy numbers. The bed of a Kurt Vise is Z -2.125", add the height of my parallels (ie +1.625 Write/Enter), and then add the thickness of my stock (ie 1.00" Write/Enter). Should be +.500". You get to the point that it becomes muscle memory and is much faster than the ways I used to do it.
It sounds complicated, but it is dead easy and I never mess it up. I also make use if the nice easy numbers. The bed of a Kurt Vise is Z -2.125", add the height of my parallels (ie +1.625 Write/Enter), and then add the thickness of my stock (ie 1.00" Write/Enter). Should be +.500". You get to the point that it becomes muscle memory and is much faster than the ways I used to do it.
D Nelson
Stainless
- Joined
- Jan 7, 2015
- Location
- Missouri Ida
I set the tools to the parallels. I program from the bottom of the work. That way nothing needs to be set at the machine set work against stop load program and run parts. Hard to mess that up
Sent from my iPhone using Tapatalk Pro
Sent from my iPhone using Tapatalk Pro
We are a job shop, it is a rarity to run more then one part. Do do have multiples, If I set the tools to the part, I would spend all day setting tool heights. I have been subtracting 2" from my part zero for years. But some people, just didn't understand the concept and I spent more time explaining the hows and whys every time they set up a part, I could have done it myself. That defeats the purpose of a hired hand! If there are no parameters to adjust, we will just keep doing it the same way and get someone else to do the job.
vmipacman
Cast Iron
- Joined
- Nov 21, 2014
- Location
- Virginia, USA
Well, my way makes sense to me with no adding/subtracting from the part height.
Put a pin (I use my haimer) in tool 1. Set that tool upset to zero. Come down on your gauge till it zeros. Now zero your z relative coord. Now set all your other tools and whatever the real. Z shows, set that as the tool offset. Basically you just referenced all your tools off tool 1, not table height. Then you zero your part using tool 1 and all other tools are good to go.
Put a pin (I use my haimer) in tool 1. Set that tool upset to zero. Come down on your gauge till it zeros. Now zero your z relative coord. Now set all your other tools and whatever the real. Z shows, set that as the tool offset. Basically you just referenced all your tools off tool 1, not table height. Then you zero your part using tool 1 and all other tools are good to go.
precisionmetal
Stainless
- Joined
- May 16, 2005
- Location
- CA
I have a Haas Super Mini Mill, and I have a Renishaw probe (but no tool setter in the machine).
Here is what I do: Using one of these ----> Pro Touch Off Gage 4- - Edge Technology ..... I set all my tools. Then I run down the tool table in the control and subtract 4" from all the values I just set. This sets all my tools to the table. Then, I keep my probe in the last pocket of the tool changer, and I have the "tool length" for that pocket/tool set to the probe length. So if I were to probe the table in Z, I get a value of 0 (zero).
Now... all I need to do is probe my part, or blank, or parallel, or vise jaw in Z, and that positive value (table surface "up" to what I just probed) gets shoved into G54 Z offset value (a positive number). Essentially, all my tool offsets have now been shifted to the point I just probed.
This system works very well (for me), and it keeps everything very simple: Tool lengths are set to the table (which NEVER changes), and G54-Z value is the distance from the table up to the origin of my part. A quick check from the table to the work offset point on the part using a 6" scale verifies that the G54-Z work offset in the control is where it should be.
It usually takes me about 15 seconds per tool to set the tool lengths, and maybe 30 seconds to subtract 4" from all the tool length values, and maybe a minute or two to probe in X, Y and Z.
Works for me.
And for what it's worth, I run a VF2 at a college where I volunteer, and it has the full Renishaw package on it. Yes... the tool setter is very slick because diameters can be checked, code can be inserted into a program to check for a broken tool, etc. But... for a basic, straightforward setup, I can set up tools and probe using my method on my SMM way faster than I can with the tool setter on the VF2. It's also simpler to verify that the Z offset value is correct because the "scale from the table" method is easier to eyeball than trying to guess where the top pad of that tool setter is.
fwiw....
PM
Here is what I do: Using one of these ----> Pro Touch Off Gage 4- - Edge Technology ..... I set all my tools. Then I run down the tool table in the control and subtract 4" from all the values I just set. This sets all my tools to the table. Then, I keep my probe in the last pocket of the tool changer, and I have the "tool length" for that pocket/tool set to the probe length. So if I were to probe the table in Z, I get a value of 0 (zero).
Now... all I need to do is probe my part, or blank, or parallel, or vise jaw in Z, and that positive value (table surface "up" to what I just probed) gets shoved into G54 Z offset value (a positive number). Essentially, all my tool offsets have now been shifted to the point I just probed.
This system works very well (for me), and it keeps everything very simple: Tool lengths are set to the table (which NEVER changes), and G54-Z value is the distance from the table up to the origin of my part. A quick check from the table to the work offset point on the part using a 6" scale verifies that the G54-Z work offset in the control is where it should be.
It usually takes me about 15 seconds per tool to set the tool lengths, and maybe 30 seconds to subtract 4" from all the tool length values, and maybe a minute or two to probe in X, Y and Z.
Works for me.
And for what it's worth, I run a VF2 at a college where I volunteer, and it has the full Renishaw package on it. Yes... the tool setter is very slick because diameters can be checked, code can be inserted into a program to check for a broken tool, etc. But... for a basic, straightforward setup, I can set up tools and probe using my method on my SMM way faster than I can with the tool setter on the VF2. It's also simpler to verify that the Z offset value is correct because the "scale from the table" method is easier to eyeball than trying to guess where the top pad of that tool setter is.
fwiw....
PM
