Reverse Counterbores

[Reko]

Good Day,

 

I have several parts that need deep counterbores on the opposite side of the part. They are for a 1.125" thru hole, and a 2.5" C-Bore gets machined on the opposite side... no way to reach them in any other operation.

 

There are approximately 55 holes per part and the C-Bore is 7/8" deep (opposite side).

 

I normally just give the operator points in the program and they can single block through and manually drop the tool down in, attach the shell-mill-style reverse c-bore tool, and manually spotface the detail. Normally, they are just spotface to a clean-up.

 

In this case, they are 7/8" deep, and there are so many holes, that doing them manually, is going to be completely inefficient.

 

My question is, has anyone ever developed a custom drill cycle to drop the tool into the hole... M00 (program stop) to attach the tool... peck the material to depth, in the opposite direction of a standard drill cycle... M00 (program stop) to remove the tool... then retract and position to the next hole where the process starts over again?

 

I have done this manually on Haas and Fanuc controllers using sub-programs, but this is an old Heidenhain that I have never operated much. I don't even know if it supports sub-programs.

 

I would like to be able to do this type of operation using MasterCam.

 

Thanks in advance for any help or suggestions.

[kccadcam]

The easiest way is to use an automatic back counterbore tool....

 

AUTOMATIC BACK SPOT FACING TOOL, REAR COUNTER BORE TOOL

 

There are a few different brands out there....

If you have a lot of holes to do,, it's worth it...

[Reko]

The easiest way is to use an automatic back counterbore tool....

 

I'd like to, but the problem is with the size of work we do here. This is a rather small diameter of 2.5" reverse c-bore for this part. We do them all the way up to 5" to 6" in diameter. The tools you are talking about are typically a 4-6 week wait (large sizes are not stocked) and the cost is, literally, in the thousands of dollars. We have a few sizes of the automatic kind, but they are not cost efficient and pretty wimpy by our standards.

 

If the size is standard, we have shell-mill style, HSS, that are attached by hand. They can be re-sharpened. If the size is non-standard, we use knockout, home-made tools.

 

I'd love to have a cycle cranked out using MasterCam, if possible.

[westerfieldc]

You could write a custome drill cycle like the what I have shown below:

 

pmisc2$ # Back Spot Face Cycle (User Option)

pdrlcommonb

pbld, n$, pzout , "F100.", e$

"M00", "(INSTALL TOOL AND PRESS CYCLE START)", e$

pbld, n$, pfspindleout , e$

pbld, n$, *sm08, e$

pbld, n$, *sg01, *tosz_a, [if dwell$, *dwell$], *feed, e$

pbld, n$, *sg00, pfzout , e$

"M00", "(UNINSTALL TOOL AND PRESS CYCLE START)", e$

pbld, n$, *sg01, *initht_a, "F100.", e$

pcom_movea

[Reko]

Does anyone know the variable name to pull "top of stock" out of the NCI file?

 

I'm really close to a custom reverse spotface cycle for a Heidenhain controller.

 

Output looks like this:

 

%0G70

;TEST

;

; TOOL-1

; 2.5" Back Spotface

N1 G90

N2 G17 T1

N3 S171 M03

N4 G00 G90 X0. Y0.

N5 Z6.

N6 Z-2.

N7 M05

N8 M00

; ADD SPOTFACE TOOL

N9 M03

N10 G83 P01 .1 P02 +1.15 P03 0.03 P04 .1 P05 30

N11 X0. Y0.

N12 Z-2. M99

N13 G00 Z-2.

N14 M05

; M00

; REMOVE CUTTER FOR RETRACT

N15 M03

N16 G00 Z6.

N17 M05

N18 G00 Z0. T0

N19 M30

 

But, line number N12 should be Z-1.75 (top of stock) not Z-2. which is my retract.

[Reko]

You could write a custome drill cycle like the what I have shown below:

 

Yes, thank you.

 

I am very close... just a few more tweaks.

 

Do you know how to extract "top of stock" from the NCI? I hope I am asking the right question there... but what I need is to have the MasterCam field "top of stock" appear on my line number N12

[CJep]

Reko,

There is a predefined variable called "tosz$" that may be what you're looking for.

[Reko]

Reko,

There is a predefined variable called "tosz$" that may be what you're looking for.

 

That is close... it produces this line:

 

N11 tosz$ -1. M99

 

What I need it to output is:

 

N11 Z-1. M99

 

Is there something I need to add with that to the post to force a "Z" and not that variable itself?

 

BTW, -1. is the number I have in the "top of stock" field, so it is pulling it from the correct field.

[CJep]

You could setup a user defined variable such as, tosz_a,

 

Then you would need to format it, fmt Z 2 tosz_a #Drilling top of stock

 

Then you would set tosz_a to grab the value in the post block, tosz_a = tosz$

[Reko]

You could setup a user defined variable such as, tosz_a,

 

Then you would need to format it, fmt Z 2 tosz_a #Drilling top of stock

 

Then you would set tosz_a to grab the value in the post block, tosz_a = tosz$

 

I must be missing something.

 

I set fmt "Z 2 tosz_a #Drilling top of stock" with the other drilling fmt statements, I defined " tosz_a = tosz$" at the top of my "Drilling Definition Section" and I used "tosz_a" as the call-up variable.

 

That still out-puts:

 

N11 tosz$ -1. M99

 

Everything else is working good.

[CJep]

Reko,

It looks like you might have to initialize it as a variable, add this with the misc variables, tosz_a : 0 #Drilling top of stock"

 

 

Can you post a copy of your custom drill post block?

[Reko]

I added the "tosz_a : 0" but it still outputs incorrectly. It looks like this:

 

N4 G00 G90 X30.7059 Y3.2273

N5 Z6.

Z1.€ N6 Z-2.

N7 M05

N8 M00

; ADD SPOTFACE TOOL

N9 M03

N10 G83 P01 .1 P02 +1.15 P03 0.03 P04 .1 P05 30

N11 tosz$ -1. M99

 

Line N6 has a strange character and line 11 is the line I want to read "N11 Z-1. M99"

 

Here is the block I'm working on:

 

p01 = 0.1 # Set 'P01' to this for REVERSE drilling

#!incdrdp # Force formula calculation

!nrefht # Force formula calculation

pdepth # Calc. the desired drilling depth

tosz_a : 0 #Drilling top of stock"

 

n$ *refht$ e$

n$ "M05" e$

n$ "M00" e$

";" "ADD SPOTFACE TOOL" e$

n$ "M03" e$

n$, *sgm1, "P01 ", *p01, "P02 ", *incdrdp, "P03", "0.03",

"P04 ", *dwell2, "P05 ", *frplunge$,e$

#n$, *x$, *y$,e$ # Move to drill location

n$, tosz$, "M99",e$ # Move down to programmed REFHT and DRILL HERE!

n$ "G00" *refht$ e$

n$ "M05" e$

n$ "M00" e$

";" "REMOVE CUTTER FOR RETRACT" e$

n$ "M03" e$

n$ "G00", *initht$ e$

n$, *x$, *y$,e$ # Move to drill location

#!refht$, !depth$, !z$

 

I'm very close here.

 

Thanks for the help.

[CJep]

Reko,

Try changing the line below in your postblock

 

n$, tosz$, "M99",e$ - change tosz$ to tosz_a

 

p01 = 0.1 # Set 'P01' to this for REVERSE drilling

#!incdrdp # Force formula calculation

!nrefht # Force formula calculation

pdepth # Calc. the desired drilling depth

tosz_a : 0 #Drilling top of stock"

 

tosz_a = tosz$ - add this line to the beginning setup in the postblock

 

n$ *refht$ e$

n$ "M05" e$

n$ "M00" e$

";" "ADD SPOTFACE TOOL" e$

n$ "M03" e$

n$, *sgm1, "P01 ", *p01, "P02 ", *incdrdp, "P03", "0.03",

"P04 ", *dwell2, "P05 ", *frplunge$,e$

#n$, *x$, *y$,e$ # Move to drill location

n$, tosz$, "M99",e$ # Move down to programmed REFHT and DRILL HERE! ******

n$ "G00" *refht$ e$

n$ "M05" e$

n$ "M00" e$

";" "REMOVE CUTTER FOR RETRACT" e$

n$ "M03" e$

n$ "G00", *initht$ e$

n$, *x$, *y$,e$ # Move to drill location

#!refht$, !depth$, !z$

 

[Reko]

CJep, thank you for taking the time to explain that to me.

 

It works perfectly. I can control everything exactly how I want.

 

I appreciate that very much.

[CJep]

Swweettttt!

 

olforum Cheers!