Tool offset setting

So the process in the manual (work off the material top) never sat right with me. And I saw the older forum post where someone made custom M Codes to zero out more like a different control. However talking to a couple guys at work today they showed me a 3rd option.

Using the tool setup menu under run and a tool setter on the table or vise ways (whatever you can reach) Go through the process of selecting each tool and wheeling down and zero out each tool (They use cheap $60 ones at work and they seem to work fine for non .0001" critical applications).

From there you can then G54 (or other) your coordinates as normal and use the tool setter to set your G54 Z wherever your CAM is setup.

Just ran through it and it worked great. Couldn't tell the difference between the part I ran last night and the one I ran today using the process in the manual and this new tool offset setup.

I figured I would share because I thought I was resigned to setting tools each program and hopefully someone else thinking the same thing will now run into this.

Thanks for the info. Going to try it out.

There are about as many ways to set tool heights as there are machinists. I usually use the set my tools to the top of the part routine because it's rare that I'm not changing a tool in a holder for a job. I have a fair amount of holders, probably close to 35-40, but there always seems to be one or two tools that need to be swapped in a holder for extra clearance, or a different drill size. So setting tools and creating a library like you are talking about is rarely going to work unless you can never disturb your tools in the holders... At least that is what I have found.

Hi Yugami, The "run, tool set" program is a very over looked option. I show all my customers . generally the response is wow, The one down side is that you need to know the difference between the tool touch off and the top of the part. the ONE big plus is if you "fat finger" a number, it will usually cut up, not down.
The "new" fangled way is to use probing ( OK, not so new but usually out of reach for a lot of "small" guys. But WAY cool. It can / will save time and money but it "aint" cheep"
You are learning at a pretty good rate. :-)

spportybob

Probing is a dream, we have that on a hass machine at work

I have an unfair advantage over a lot of the home cnc guys. I'm a manufacturing engineer with lots of educational support from machinists.

Being that probing has come up, there are cheap probes out there, under $200, and I was wondering if the Milltronics software would support adding one into the machine. I see parameters in my machine related to probing, so would/could it be a matter of attaching a probe, turning on some parameters and have the ability to probe edges, corners and bores? I'm tired of wigglers and electronic edge finders and can't bring myself to spending $400 on a Haimer 3D taster.

The probing that Yugami is talking about runs about $6K. You can add the Renishaw probing to most any Milltronics. And like Haas it is an option.
When set up properly the probing can and will pay for it self in short order. With the right macros t run it, it can not only help with part setups but can be used for part inspection as well. saving the "test data to a down loadable file/ if you are a busy shop. these files help meet certain ISO specs. well worth the money.

Not sure what kind of "probe" you can get for $200.

sportybob

I know what Renishaw style probes are and that's way out of the price range, my old mill is too shot to hold those types of tolerances anyway. I'm just thinking to replace a wiggler and have some automatic possibility of setting G54. As for probes, this one is something I have seen:

https://www.ebay.com/itm/CNC-3AXIS-D...YAAOSwbtNaEzTD

Maybe if they have one that has normally open contacts, you could wire it to an input and write some macros to do that.

sportybob

Quote:

---

Originally Posted by sportybob

Maybe if they have one that has normally open contacts, you could wire it to an input and write some macros to do that.

---

Hey bob, how does one monitor an input in a macro? I have a tool offset probe I made and want to try and wire in to input 11.

The easiest way is to go to "F6 display, F4 DIAG and look at what the input is doing. depending on the software version you may have to do the PROTO3 level 3 thing to get to DIAGS. depending on the software version, either a 0 (off) 1 (on) white dot (on) black dot (off)

one would need to know "what" 11 you are referring to. X, Y Z A or ????

I am going to assume that you are using some kind of probe and do not have the macros that are part of the "probe package" Ask the probe supplier to provide the macros for the Milltronics. ( or any other machine) :-( A lot of the cost in probe systems is because "someone" knows Macro programming, and has spent considerable time in developing the macros for each machine control.

Not to be an ass, but suppose you spend 1 year developing a product and you sell it for X $, some one comes behind you and copies YOUR product and then sells it for less money and you did ALL the work. not right and fair.

All the info is in the "parametric" programming section of all Milltronics CNC programming manuals.

as an example here is an arced and curved 5 bladed fan. (From the manual)
P2=0
N2
N1
P1=.5
P140=.1
G31
G0 X[P1] Y0
G1 Z0
G3 R[P1] AA0 AB45 Z[[.5-P1]/5]
G31
P1=P1+.1
IF P1 LE 2 GOTO 1
P2=P2+72
G68 AA[P2] I0 J0
IF P2 LT 360 GOTO 2


( A lot is going on the 13 lines of programming) but it gives you an idea of what is possible

Macro programming is not "easy" but it is under stand able. Boolean algebra ( If, Then, Or, Else) is a requirement.

I know you are looking for the cheap and fast "answer" but, That would be "plagiarizing" someone else's work. It all falls back on "What's right and What is Fair" IMHO.

I don't mind sharing what I know, but I will NOT give away someone's else work. with out their permission.

To ( kind of ) quote an OLD expression, " give a man a fish, feed him for a day, Teach a man to fish , feed him for life".


See the manual. As a teaser, ( Teach a man to fish)

SECTION SIX - PARAMETRIC PROGRAMMING
INPUT The INPUT statement is used for data input from the front panel.
Example: INPUT (X START POSITION) P1
The operator will be prompted to input data.
The operator can use the data displayed by pressing the ENTER key. If ESC is pressed during an input statement, the program will be terminated.
The HDW command can be used to enter the handwheel mode during a program. A
comment may be added to prompt the operator during the HDW command. HDW is
ignored when verifying a program.
Example: HDW (TOUCH THE TOOL TO THE PART) prompts the operator with the following message.
The operator presses the <enter> key after handwheeling the machine. If <esc> is pressed during handwheeling, the program will be terminated.
To manually set and clear input/output pins, refer to the following.
CLR Clear an output pin.
Example: CLR X7 (clears X output #7)
SET Set an output pin.
Example: SET Z3 (sets Z output #3)
34 6
SECTION SIX - PARAMETRIC PROGRAMMING
PULSE0 Pulses an output pin.
Example 1: PULSE0 Z10 (clears Z output #10, delays for the number of milliseconds specified by the MISC parameter PULSEx pulse delay(ms) then sets output Z10)
Example 2: PULSE0 X2 P3.5 (clears X output #2 and delays for 3.5 seconds, then sets X output 2)
PULSE1 Pulses an output pin
Example: PULSE1 X5 (sets X output #5 delays for the number of number of milliseconds specified by the MISC parameter PULSEx delay(ms) then clears output X5)
STO STO is similar to the SET command, except the outputs are consecutive. There are twelve outputs on each axis.
Example: STO20 (sets Y output #8 or the 20th output)
CLO CLO is similar to the CLR command, except the outputs are consecutive.
Example: CLO25 (clears Z output #1 or the 25th output)
PIN PIN refers to a pin. X axis are 1000’s Y axis are 2000’s, Z axis are 3000’s, etc.
PIN X Axis Y Axis Z Axis 4th Axis 5th Axis 6th Axis in1 1000 2000 3000 4000 5000 6000 in2 1001 2001 3001 4001 5001 6001 in3 1002 2002 3002 4002 5002 6002 in4 1003 2003 3003 4003 5003 6003 in5 1004 2004 3004 4004 5004 in6 1005 2005 3005 4005 5005 in7 1006 2006 3006 4006 5006 in8 1007 2007 3007 4007 5007 in9 1008 2008 3008 4008 5008 in10 1009 2009 3009 4009 5009 in11 1010 2010 3010 4010 5010 in12 1011 2011 3011 4011 5011 out1 1012 2012 3012 4012 5012 6012 out2 1013 2013 3013 4013 5013 6013 out3 1014 2014 3014 4014 5014 6014 out4 1015 2015 3015 4015 5015 6015 out5 1016 2016 3016 4016 5016 out6 1017 2017 3017 4017 5017

( that did not copy from the manual as "shown".)

see the manual.

sportybob

Hrm you're section 6 is very different from mine, no wonder I couldn't figure out a starting point.

Macro programming won't be a huge problem. And the hardware is all done already. Wireless and everything. I need side people's to work on while the big ones are frustrating me.