Newb check in. Drilling and Milling Q.

[countryguy]

In the images from this Site:
http://www.cnczone.com/forums/dolphin-c ... ost1773760


I have a new controller- I have been using and LOVING your setup. Now, I've learned about tool length offsets I think. This Q. is when you have drilling ops and Milling ops together as I do on the simple part in the URL above.

Since I do not have enough travel for all the parts in Z- length I figured I would :
Split my CAM to output G code for:
1:
a) Drilling ops. My Drill tool 1. Will also be the Ref tool. Thus on the length offset for Tool 1 I will have 000.
b) for Drill 2. Simply measure and F10 the value.
c) Run , Graph and check it all will go thru. I loove Graph to quickly check for issues.

And here is where I get cloudy.... I need to move the knee up. So I move it up. then what? ( I keep watching the Video too
Should I just reset the Reference tool to something smaller as the Ref tool is now way too long? OR did I miss the whole concept of the Video?
2:
a) milling ops. Input my Mill tool 1: Just set it as Ref tool. set it as tool 3 and offset 000
b): Measure Mill tool 4. Get the tool length diff.
run the part?

Where I get confused is the relationship between moving the table back up and reference tool and my tool offsets for the job. Hope this makes some sense.

Best,
JJ / CG.

[cnckeith]

there are several ways to handle the limited z travel of a typical knee mill.
one basic way is to create a part program to do all the machining with the knee at one Z position.
and then drop the knee, reset just the Z part zero (wcs) and then perform all the drilling operations at that new z height with another program. a more sophisticated way is to join those two programs and put in a stop and wait for operator which prompts you to drop the knee at the appropriate time , then switches to a new WCS position that matches the dropped position (same X and Y, just different Z) . guys that do this typically have a Scale on the knee (connected to the control) so they can drop the knee to an exact position. adding a scale is easy and cheap and if you own a knee mill i highly recommend it.
other tricks that guys who do ALOT of drilling will do is... put drill stops on the drill bits so they can locate the drill bit to the same approximate position in the same drill chuck. you can usually group a size range of bits like this, obviously you can't put a regular 1/2 bit in a drill chuck at the same length as a 1/8" drill bit. and depending on the type of drilling you can buy jobber drill bits which are short for those jobs that you don't need the length of a typical drill bit. this helps out with z height limitations as well. the drill bit stops allow you to change the tool from the drill check and use the same offset value.. that way you have one offset value for a particular group of drill bits that you can put in the drill chuck at the same position.
ive attached instructions on how to add a scale to the knee

[cncsnw]

You can also do it more or less as described in the original post.

Treat it like two separate programs, with two separate setups, using two entirely separate sets of tools.

You declare one of the drills to be the reference tool for the first setup. You set Z reference with it, and all other tools in the first setup are measured in comparison to that reference tool. You then set X, Y and Z part zero, using any one of the first batch of tools to set Z axis part zero. You run the first program.

Then you raise the knee, and choose one of the milling tools, or something of similar length to the milling tools, to be your reference tool for the second setup. You set Z reference with the new reference tool; make sure its height offset is 0.0000, and measure the rest of the second batch of tools in comparison to the new reference tool. You set a new Z axis part zero using any one of the second batch of tools. You run the second program.

As long as you don't mix tools between the two setups, and as long as you reset Z axis part zero whenever you change from using one setup to using the other, this will work just fine.

[countryguy]

Thanks guys! Good info. I appreciate the quick responses too. I think a scale on the knee would be a really nice touch and end up being really functional. Great idea. I'm interested in the WCS part of Keiths post. That seems a creative way to also help make it "quick". With a Knee Scale it would let me setup and move between the two operations precisely as needed. Again... I love this software.

Sidebar- when I set 0,0,0 and have a part loaded - Say I shutdown for the night- When I come back and power up, cycle to home- Is 0,0,0 where I left it? I mean if the part is still on the table can I just load the program and hit cycle start ?

Have a great week everyone.
Jeff

[cnckeith]

yes you can set the machine up to do just that. there are several ways to "home" the machine each time you power up so it will remember your part x,y,z zero position (and all the other WCS positions you have setup )
as you could imagine this is a real time saver.
automatic homing is available if you have limit switches (or home switches) installed. each time you power off and power back up the machine will ask you to press cycle start and it will automatically home out and find its position.
another way to home the machine that is switchless ...is called "home to marks" this is a semi automatic homing technique. i really like this one since i don't need any limit or home switches to repeat to the exact position after a power cycle.
either method doesn't actually use the switch or the mark to set the home position.. in both cases the marker pulse on the encoder is used.. once per revolution a special pulse on the encoder (the marker plulse) is sensed by the control... so the same home position can be determined as long as you get the machine to the same position to within one revolution of the servo motor.. this can be easily done with a physical mark on the machine that you can eyeball line up or with a regular old limit (home) switch ( or prox swtich) that will do that for you.
there is also a "park" feature in "shut down" menu , that will park the machine tool close to the home position so its ready to home out when you power back up.
I use a G30 command with 'home to marks' before shut down. g30 is just a position based on machine coordinates. i set the G30 to go to the x,y,z that i used when my axis marks are lined up... that way i don't have to eyeball the marks up the next morning to home out the machine.
if i forget to issue the g30 before shut down..its no big deal..i just jog each axis until the marks are lined up and press cycle start and the machine homes out from there finding the marker pulse automatically, it just takes a few seconds and i'm ready to go cut some parts and my zero position and tool offsets are still the same as when i shut the machine off. pc of cake.

[countryguy]

Still having issues but 1 run did go fine. Now I'm all buggered up. Reading this and a few other posts. Just need time to sit , read, play on some scrap making a circle or two.
http://www.cncsnw.com/OLEM.htm

[cncsnw]

If after sitting, reading, and doing some careful simple experiments, you are still having problems, then you need to post specific details.

Tell us what your CNC program actually says; what values are in your tool offset library; and what DRO position display and status window (in the upper right corner) show when a tool is cutting at the wrong depth.

For example, if you come to the point in your program where Tool #2 is supposed to rapid down to a 0.100" clearance, but in fact it is continuing on down to contact the part you should note:
1) Does the DRO position show something between 0.0000 and 0.1000, or does it show something significantly higher, even as the tool reaches the part?
2) Does the status window say "T2 H2", or does it say, perhaps, "T2 H0" or "T2 H--"?
3) Does the current line of the program indeed say something like "G0 Z0.1", or is there some other Z value there?