We have a commonly used tool (T03) that needs different offsets/comp when the programs change. I'm looking to add a section in the program that will write the tool comp directly from the program, which will lessen one more chance for operator error. Our machine is a Brother S700 with a CNC-C00 Control. Any help would be appreciated. Have a nice week!
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:
How to write tool comp from the program
- Thread starter eztrakman
- Start date
- Replies 20
- Views 3,249
aj
Hot Rolled
- Joined
- May 12, 2006
- Location
- Burlington, North Carolina
If I understand your question, sinha is correct. You can call any tool with any offset that isn't being used by another tool.
Example:
G43 Hxx (Tool height)
G41/G42 Dxx (Tool diameter for cutter comp)
xx can be any number your controller supports and isn't being used by another tool. Just put whatever numbers you want in offset xx and the controller will load them when you call them with H and D.
Example:
G43 Hxx (Tool height)
G41/G42 Dxx (Tool diameter for cutter comp)
xx can be any number your controller supports and isn't being used by another tool. Just put whatever numbers you want in offset xx and the controller will load them when you call them with H and D.
Matt@RFR
Titanium
- Joined
- May 26, 2004
- Location
- Paradise, Ca
Either do the above, or:
#11001 = 2.539 (writes 2.539" as the length of T1)
#11001 thru 11099 is tool length T1 thru T99
#10001 thru 10099 is tool length wear
#12001 thru 12099 is tool radius wear
#13001 thru 13099 is tool radius
We use both methods on a daily basis, just be careful with using multiple H offsets for the same tool.
#11001 = 2.539 (writes 2.539" as the length of T1)
#11001 thru 11099 is tool length T1 thru T99
#10001 thru 10099 is tool length wear
#12001 thru 12099 is tool radius wear
#13001 thru 13099 is tool radius
We use both methods on a daily basis, just be careful with using multiple H offsets for the same tool.
Success
Thanks for the replies. Today I learned all about G10. This is what I added to my programs, tested and worked.
(******** TOOL OFFSETS ********)
G90 G10 L11 P03 R-.0500
G90 G10 L12 P03 R-.0125
(L10 = length offsetting **DO NOT MODIFY USE METROL PRESETTER**)
(L11 = "H" wear offsetting, P = offset number, R = value)
(L12 = "D" geometry offsetting, P = offset number, R = value)
(L13 = "D" wear offsetting, P = offset number, R = value)
(******** TOOL OFFSETS ********)
M01
Thanks for the replies. Today I learned all about G10. This is what I added to my programs, tested and worked.
(******** TOOL OFFSETS ********)
G90 G10 L11 P03 R-.0500
G90 G10 L12 P03 R-.0125
(L10 = length offsetting **DO NOT MODIFY USE METROL PRESETTER**)
(L11 = "H" wear offsetting, P = offset number, R = value)
(L12 = "D" geometry offsetting, P = offset number, R = value)
(L13 = "D" wear offsetting, P = offset number, R = value)
(******** TOOL OFFSETS ********)
M01
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
I'm curious about this. I have 5 tools that always stay in the magazine and are used on almost every part and program I run. The only time I change the length offset or radius comp values are when I replace the tool. What is going on that you need to change those values for each different program?
Matt@RFR
Titanium
- Joined
- May 26, 2004
- Location
- Paradise, Ca
I can't speak for the OP, but when working to tenths on pretty much everything, we use multiple D and sometimes H offsets for certain tools in each program, let alone from one program to another. Let's say one endmill is finishing a tight tolerance (dia and depth) counterbore and a tight tolerance feature wall and floor that has to blend with another tool's length. I would program that tool with two D offsets and two H offsets so all of that could be tuned independently.
A program we're running right now has 8 tools and a total of 7 additional offsets being used, and all of the offsets have different numbers in them to get everything running dead nuts.
+/-.005 stuff, sure let one feature be .0005" big and another be .0005" small or whatever. That doesn't work for us though.
T03 is a .125 Harvey Tool 300deg undercut ball deburring tool. We're using this to deburr the top and bottom of the holes drilled in the part on a radial surface. I had to make different WC offsets for the top/bottom, so it can be adjusted easily, especially the Z. When we change over from part to part, the hole dia changes as well, along with the chamfer size.
When I wrote the program in MasterCam, I used a simple X0. Y0. WC for the toolpath, which gives me the basics.
Out at the machine, I still need to tweak it it a bit. This option does that.
I know if MasterCam was fully setup for our 5axis Nikken, this would go number for number.
MasterCam gives an option for tool comp (Tip or Center). I need something in between.
Imagine the first option for cutting contact was at 3o'clock. The second option was at 6o'clock. I need option three at 4:30.
I'm just learning how to do all this, so over time, things may change, but for now...it works.
Hope that clears up the confusion.
mjk
Titanium
- Joined
- Oct 20, 2005
- Location
- Wilmington DE USA
"I'm curious about this. I have 5 tools that always stay in the magazine and are used on almost every part and program I run. The only time I change the length offset or radius comp values are when I replace the tool. What is going on that you need to change those values for each different program?"
My Z0 reference could be the top of the vice jaws one day or a special fixture the next
My Z0 reference could be the top of the vice jaws one day or a special fixture the next
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
Thanks for your explanation. I suspect the OP is doing it for similar reasons.
If a one-off or really low volume part, I'd do the same. For my repeat jobs, if I'm seeing variations from feature to feature, I'll tweak the program so all features are on size with just one offset. Less data to manage at set-up time.
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
mjk
Titanium
- Joined
- Oct 20, 2005
- Location
- Wilmington DE USA
"Does that mean you set your tools off different reference surface as jobs/setups change?"
Yes
90% of my work is off of special fixtures.
All programs have notes that tell me where Z0 X0 & Y0 are located evan if fixture is marked
Some jobs repeat about once every year, many every 2 years.
Oh and to make it more of a "Why is he doing that!!!!!"
I use G44 not G43
Benefits of working by myself
Mike
Yes
90% of my work is off of special fixtures.
All programs have notes that tell me where Z0 X0 & Y0 are located evan if fixture is marked
Some jobs repeat about once every year, many every 2 years.
Oh and to make it more of a "Why is he doing that!!!!!"
I use G44 not G43
Benefits of working by myself
Mike
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
nscele
Aluminum
- Joined
- May 30, 2007
- Location
- Australia Qld
I hope Mike is not actually touching off every tool used on every new setup?
mjk
Titanium
- Joined
- Oct 20, 2005
- Location
- Wilmington DE USA
"I hope Mike is not actually touching off every tool used on every new setup?"
Yes, and without a Reinshaw probe, just a (2" zero set) forget the brand name
When I first started with a vmc my mentor went thru the logic behind where your reference Z0 could be, and use of G43 vs G44
The time logic behind G43 vs G44 is not typing the "-" sign.
Yes I'd agree that if all tools were say referenced off the table with the work surface being the shift difference, keeping those tools at the ready would save a time.
Evan with repeat jobs, I find the setup process is the time I mentally review any quirks in the job.
The machine is warming up, it takes maybe 30 second per tool to measure, a few seconds to pop in the pocket.
Evan if I load the full magazine, that's maybe 20 minutes. If I have a job that requires 20 tools, my profit will more than cover an extra 20 minutes of time
The condition the op is discussing isn't something I have to deal with, I'm the programmer and operator
Yes, and without a Reinshaw probe, just a (2" zero set) forget the brand name
When I first started with a vmc my mentor went thru the logic behind where your reference Z0 could be, and use of G43 vs G44
The time logic behind G43 vs G44 is not typing the "-" sign.
Yes I'd agree that if all tools were say referenced off the table with the work surface being the shift difference, keeping those tools at the ready would save a time.
Evan with repeat jobs, I find the setup process is the time I mentally review any quirks in the job.
The machine is warming up, it takes maybe 30 second per tool to measure, a few seconds to pop in the pocket.
Evan if I load the full magazine, that's maybe 20 minutes. If I have a job that requires 20 tools, my profit will more than cover an extra 20 minutes of time
The condition the op is discussing isn't something I have to deal with, I'm the programmer and operator
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
If it works for you then it's cool.
When I first had a CNC mill placed in front of me back around 1982, I was taught the same as you and followed that process for a year or so before changing to setting tools to a common reference to save time and minimize error potential.
When I first had a CNC mill placed in front of me back around 1982, I was taught the same as you and followed that process for a year or so before changing to setting tools to a common reference to save time and minimize error potential.
