Heule Chamfer Tool custom drill cycle post

[Kduhn66]

We're trying to use a tool from Heule Corp called the snap tool that chamfers the top and bottom of a hole. The problem is program a part with multiple holes you have to have the required moves for each hole. A drill cycle would work but not as efficient and the recommended.

Here's an example of chamfer material 1/4" thick

The tool requires a move to get the insert close to the part. Feed down to cut the top. Rapid below the bottom of the hole to clear the top of the insert. then feed back up to chamfer the bottom. Then rapid out of the hole. I am using X4 and X5 on Haas machines.

( CHAMFER )

N136 T15 M6

N138 G0 G90 G54 X-1.9325 Y-5.425 S2500 M3

N140 G43 H15 Z.1

N142 M98 P1001

N144 X-.5475 Y-5.425

N146 M98 P1001

N148 X.8375 Y-5.425

N150 M98 P1001

N152 X2.2225 Y-5.425

N154 M98 P1001

N156 X2.2225 Y-1.425

N158 M98 P1001

N160 X.8375 Y-1.425

N162 M98 P1001

N164 X-.5475 Y-1.425

N166 M98 P1001

N168 X-1.9325 Y-1.425

N170 M98 P1001

N172 G80

N174 G80

N176 M5

N178 M9

N180 M99

N182 M30

 

N184 O1001

N186 G00 Z-.2

N188 G01 F10 Z-.380

N190 G00 Z-.57

N192 G01 F10 Z-.380

N194 G00 Z.1

N196 M99

 

I know it may be a little rough but from what I think would be right it should move to each location then to the sub and do the required Z moves. Go back the main then move to the next location and so forth. This is a small program with only a few holes. We have 4 sided tombstone with about 24 holes per side.

Does anyone know how to edit a post and create a custom drill cycle for this or is what I'm doing about the best way? I've never edited a post before and haven't figured out the custom drill cycles. The parts we do are pretty easy by todays standards.

Any help would be greatly appriciated.

 

Thanks

Kyle D.

[EX-wccprogrammer]

The subroutine approach will work, but if you do different parts, there is a lot of editing required. I like the custom drill cycle, personally. The less I have to edit, the better.

You should know, though, that a custom drill cycle is more than just post work. You also need to edit the text definitions in the control to identify the custom cycle and the parameters that it uses to function. Or you will forget where to put the data. HTH

[Kduhn66]

That's kinda what I'm leaning towards. Editing post and the other files is out of my skill right now. I got in contact with my mastercam reseller and In-house solutions. Hopefully they can figure it out. Too much programming to do manually.

[Craig-B]

If you have custom macro on your machine, you can achieve this by writing a macro and then just move to position and call the macro. All in all about the same work as doing the post edit.

[Jimmy Wakeford from Barefoot CNC]

Here is a custom cycle I made for using heule tools to chamfer different depths:

 

pmisc2$      # Canned Misc #2 Cycle 
hole_cnt = 1
p_get_cham
n$,"(",*hole_cnt,")",e$
n$,*x$,*y$,"(",*hole_cnt,")",e$
chm_z = top_chm + chm_clr
n$,"G0",*chm_z,e$
chm_z = top_chm
n$,"G1",*chm_z,pfr,e$
chm_z = bot_chm - chm_clr
n$,"G0",*chm_z,e$
chm_z = bot_chm
n$,"G1",*chm_z,e$
chm_z = refht$
n$,"G0",*chm_z,e$

pmisc2_2$    # Canned Misc #2 Cycle 
hole_cnt = hole_cnt + 1
n$,*x$,*y$,"(",*hole_cnt,")",e$
chm_z = top_chm + chm_clr
n$,"G0",*chm_z,e$
chm_z = top_chm
n$,"G1",*chm_z,pfr,e$
chm_z = bot_chm - chm_clr
n$,"G0",*chm_z,e$
chm_z = bot_chm
n$,"G1",*chm_z,e$
chm_z = refht$
n$,"G0",*chm_z,e$



chm_z : 0
hole_cnt : 0
chm_clr : 0
top_chm : 0
bot_ chm : 0
fmt Z 1 chm_clr
fmt Z 1 top_chm
fmt Z 1 bot_chm
fmt Z 1 chm_z
fmt "HOLE="4 hole_cnt
p_get_cham
chm_clr = peck1$
top_chm = dwell$
bot_chm = shftdrl$
#*chm_clr,*top_chm,*bot_chm,e$

 

...and the custom text:

[misc2]
1. "Custom Chamfer"
2. "Feedrate"
3. "Top Cham Z"
4. "Initial height"
5. "Reference height"
6. "Depth"
7. "cham clearance"
8. ""
9. ""
10. ""
11. "Bot Cham Z"

[Kduhn66]

So this Post edit looks like what I need. I found the pmisc2$ and the pmisc2_2$ lines and I replaced them with the new stuff. The next block off lines I'm not sure where they go so I put the after the pmisc2_2$ block of codes. I found the misc2 texting towards the end of the pst file and replaced it with the new text. Changed the name to chamfer tool since pmisc2 was the rigid tapping cycle. When I do a drill cycle and use this cycle it shows up as the chamfer cycle and puts moves in the nc program and it looks like it wants to work but it throws an alarm. Do I need to edit the MMD file as well?