Someone please help before I loose my mind!

[saabaero]

I've had my Tormach for a couple of months now and have been playing around learning it. I admit I am new to CNC machining (CAM and "G" code) but have been around 3D CAD since its introduction and have built a number of multi-axis stepper driven 3D trimmers. So I didn't expect to have much trouble adjusting to fixture reference systems and tool tables as such. However getting tool heights to work in any logical manner seems to be beyond me.

At first I just played with setting the tool tip location to the work piece without having a tool table set up. I have a dial indicator type tool height setter so I'd just zero the setter and key in its offset of 2" into the "Z" and proceed to run a program. On more cases than I care to think about I either buried or came close to burying the tool into the workpiece. So after having had enough of that I decided to set up my tool table and do everything by the book.

I referenced all of my tools to my touch probe (T99) using my height gauge and double checked each of them with the tool height setter on the mill. Each one was with tenths.

So today I go to machine a part with a program created in Sprutcam and posted with the latest Tormach post.

I start by referencing the machine to "Home", Install the touch probe and set my "X" and "Y" zeros and then use the "Z" probing window to set the "Z" height to zero. I then inserted my tool, keyed in the tool number, bumped it up to my tool height setter and it was within tenths of the 2" offset. (Perfect!) I had started to pocket out this area last night so this start pass should have cut air but instead it started to plunge into the material and remove material. I quickly hit the "pause" and then "cycle stop"buttons and reinserted the height checker. Instead of reading 2.000" as before it read 2.2746"

I then repeated the whole process with the touch probe to reset the zero, reinserted the tool and checked it to the height checker. Right on again! Hit the "cycle start" button and paused the machine before the tool got to the surface. I inserted the tool checker and it read 2.2749". I repeated the process two more times and everything is fine until I hit the "Cycle start" button then the height shifts to the 2.2746-9" value. And yes, the correct tool is being selected by the program.

As near as I can tell its not related to missed pulses or motor slippage as the new "Z" height after the program is started is consistently within tenths. Also it appears that as the program starts I can see the "Z" readout jump to a new value instantly as the "Z" axis starts to move. Almost like it is getting reset by the program to a new value.

My modal codes are: G15 G1 G17 G40 G20 G90 G94 G54 G43 G99 G64 G97 (don't know what a G97 is!)

The first lines of the program are:
N20 G90 G17 G40 G80 G49
N30 G20 (Inch)
(Hole machining)
N40 M998
N50 T7 G43 H1 M6
(1/2" x 1/8"r Carbide Bullnose)
N60 S3000 M3
N70 G0 X2.6 Y-2.5 Z0.561
N80 G0
N90 G0 Z0.039
N100 G1 Z-0.086 M8 f2

Sorry for the long post but I am at wits end!

[wvines]

>> N50 T7 G43 H1 M6

You are selecting tool 7 but applying the offset from table entry 1.

You probably want this instead:
N50 T7 G43 H7 M6

[saabaero]

wvines,

Thanks for your speedy reply.

I'm not sure I understand what the "H" code stands for but I guess I was under the impression that by the CAM software specifying the "T7" that the CAM software referenced the tool tip to zero and that the control program would use the tool height offset from the controller tool table for the tool# specified. I was thinking that the tool height in the CAM tool table was just for reference so one could select the correct tool that would be referenced by the "T" code If you know what I mean.

Could you explain why the values from both tool tables are used as it seems redundant.

I'm sure that there must be a good reason and that I just don't understand enough yet for it to make sense.

NTL - You may have just saved me from a trip to the insane asylum. I guess I have a lot to learn yet!

***something just struck me - Is the T# only used for selecting the tool for the tool changer and the H# used for selecting the tool offset from the controller tool table?????***

[wvines]

There are two things going on in the block.

First the "T7 M6" directs the toolchanger (you!) to put a new tool into the spindle.

Second the "G43 H7" tells the control to lookup position 7 in the tool table and apply the Z offset from that entry.

There may be cases where the T parameter and the H parameter should be different, but they make my brain hurt so I don't think about them anymore.

[saabaero]

That certainly makes a lot more sense to me now. I guess when I decided to set up my tool table in the control program I should have gone back one step farther and set up a matching tool table in my CAM software and re-generated the toolpaths. I can see where the tool information in the CAM software is necessary to certain toolpath calculations such as when using ball endmills to machine 3D contoured surfaces.

Moving from manual machining to CNC in my home shop has certainly proven to be a lot more of a challenge than I ever expected. But I am certainly enjoying the learning process. It is frustrating at times but I'm sure some day I'll look back and laugh. In the meantime I hold my breath every time I press the "cycle start" button.

Thanks so much for all of your help!

[HMB3000]

I just find it faster and easer not to use the tool tables. I have modify my post so it does not output any G28,H,D,G43....Just load the tool touch offset set zero and run....This works for me as the work I'm doing in my Tormach...I have found it faster to change part and run one tool at a time....Then change tool and run one part at a time....Also if I forget to load offset then no issue with zero value

[stedgar]

In line N50 of your program it sets the tool hieght to the hieght of tool 1 (
H1). what is the length of tool 1 compared to tool 7? Sprut has a bad habit of not using the correct tool hieght numbers. Double check those. I have gotten into the habit of using notepad to read teh g-code checking those kind of things.

Good luck
Steve
Austin Texas

[saabaero]

Actually, I can't blame this one on anyone but myself. I went in and manually changed the "T"# in the NC file once I set up my tool table up in the control software and didn't realize that the "H"# had to match. I thought the tool height and tool was both selected by just the "T"#.

This one drove me crazy because the machine seemed to have a mind of it's own and no matter how many times I reset the "Z" tool tip origin it never maintained that value and would just change to something else on its own.

I have to admit that the whole tool offset issue makes a whole lot more sense to me now and that I am extremely grateful for all the help I received here.

[mactec54]

Hi saabaero

I'm surprised the control would even run as it is not meant(Most Will Not Run) to run if you have T7 H7 not matching the Control software needs to be fixed so this can not happen looking at your Gcode output from your cad/cam looks to be a mess as well PM
me & I will help you get it right

The G97 is constant surface speed control cancel

[HMB3000]

you can have many hight offset H # for the same tool...you just can't change the H# without using G49 and going to a G28 move first...this is done when say you have more than one fixture offset of part on table

[mactec54]

Hi HMB3000

Saabaero is just learning to get things going he does not need to know about what you can do he just wants to be able to get going very basic without crashing

[HMB3000]

Originally Posted by saabaero I'm not sure I understand what the "H" code stands for

H=Hight Offset...

Originally Posted by mactec54 Hi HMB3000 Saabaero is just learning to get things going he does not need to know about what you can do he just wants to be able to get going very basic without crashing

Mactec in the last few years as an Appoved Independent Consultant for Tormach... I have help a lot of people get started...I will always explain where you can get to when learning the basic. This is to let them know why they should think a certan way and look at thing.