Slow drilling

[kstrauss]

I use the Mach3 post.
When peck drilling, the retraction is fast but the plunge back to the previous depth is at feed rather than rapid speed (G1 versus G00). Many of my projects require drilling dozens of deep holes so the slow plunge is a significant waste of time. Is there any way to improve things?

[adze_cnc]

The naïf in me says, "increase the plunge rate in your tool setup if you want the drill to plunge faster". As an example I changed the "plunge rate" to 200 inches/min and lo and behold the G1's get F200 added by my post-processor---not that my machine can actually do that speed.

Code: Select all

 N0G90
 N10(End Mill (0.125 inch) full depth)
 N20M6T5
 N30M3 S18000
 N40G0 X0.0164 Y0.0829 Z1.6400
 N50G1 Z1.0860 F200.0
 N60G0 Z1.3240
 N70G1 Z0.9480 F200.0
 N80G0 Z1.3240
 N90G1 Z0.8100 F200.0
 N100G0 Z1.3240
 N110G1 Z0.6720 F200.0
 N120G0 Z1.6400

[Leo]

But then you are "drilling" at 200 IPM

[Leo]

I know what you are looking for. I write G-code on more expensive machines and there are options available that we do not have with Vectric or Mach3.

It is not all that hard to write the code to peck drill.

Basically you want to retract all the way out, then rapid in to something above where you just drilled to, then feed to the next depth.

I usually write one peck depth with retract and rapid in and drill depth. Then I copy and paste a bunch of blocks then edit the depths accordingly for each depth.

Only need to write for one hole.

Move tool to new location and copy / paste the hole pattern to a new location.

You can use Vectric for the locations and edit in your drilling pattern.

Whenever I post about writing g-code it's not usually well received. I'm ok with that, but I don't see that particular peck drilling option in Vectric. Seems like it would be easy to add. Maybe the post can be edited to make it happen.

[kstrauss]

Yes, the ability to use a G73/G83 "canned cycle" would be ideal. I have often edited the Gcode to do such but it is a pain and prone to typing errors. It would be great if Vectric would modify their code generation to output routines for things like drilling that use named parameters like they allow [T] for tool change. That way the user could modify the post to do what is desired.

I said that I was using the Mach3 post. Actually I have modified the standard Mach3 one to work with PathPilot and handle things such as coolant on/off, G30 before tool changes, zero spindle RPM for drag engraving, etc.

Cut2D does a good job as a low cost and easy to learn CAM package. It is a shame that Vectric doesn't change a few things so that users can make it even better.

[Leo]

In defense of Vectric, they DO listen to us. Often times the upgrades are of characteristics the users are asking for.

As to the drilling cycles, I honestly have not seen much posting in the 7 years I have been on the forum about the drilling cycle. YES, I agree it would be a nice to have, but I am sure Vectric has larger requests than the drilling cycle.

I don't expect to see that change in future releases, but, if it does change, I would love it as well.

Yeah, it's a pain to write the code, and we would love to click a button in the CAM. But the code for a peck drill is really pretty easy to write and prove out. It can be done in Excel with a little math functions, then copied and pasted as text.

[kstrauss]

Judging from the questions here I suspect that drilling is of very little interest to the typical Vectric user. As a retired software developer I understand that you need to satisfy the wants of most customers rather than special interests, some changes that appear trivial are not and that every change requires extensive testing. That said, changing to rapid feed to the previous depth should not be difficult. Since the information dialogs are already there, adding canned cycles would be icing. Now about tapping cycles...

Do you know if Vectric developers monitor this forum or would it be best to contact them directly?

[adze_cnc]

I wonder if it is possible to implement the rapid G0 move via modifications to the post-processor?

[kstrauss]

Not that I can see. It appears that only a portion of the final Gcode -- tool change commands for example -- is produced entirely by the post. Other parts of the total program appear to be produced by invoking primitives in the post such as RAPID_MOVE and FEED_MOVE. The post doesn't know whether a drilling sequence or a normal cutting sequence is being produced so I don't see how I can get the desired result. I'd love to be proven wrong...

[adze_cnc]

Perhaps: FIRST_PLUNGE_MOVE, PLUNGE_MOVE, RETRACT_MOVE, and DWELL_MOVE are sections to check out?

Steven

[Leo]

Judging from the questions here I suspect that drilling is of very little interest to the typical Vectric user. As a retired software developer I understand that you need to satisfy the wants of most customers rather than special interests, some changes that appear trivial are not and that every change requires extensive testing. That said, changing to rapid feed to the previous depth should not be difficult. Since the information dialogs are already there, adding canned cycles would be icing. Now about tapping cycles...

Do you know if Vectric developers monitor this forum or would it be best to contact them directly?

They do monitor, but a friendly direct contact never hurts. I like canned cycles. RIDGID TAPPING, would be nice for the 2-3 people in the Vectric world that would use it. I wonder if I can tap at 20,000 RPM's

[kstrauss]

Thanks you for your suggestions.

After editing my post and running a quick test, it appears that FIRST_PLUNGE_MOVE is invoked for each downfeed of the drill bit. That is, Cut2D does a RAPID_MOVE to the hole location followed by a FIRST_PLUNGE_MOVE to the depth of the first peck. Then a RETRACT_MOVE followed by a FIRST_PLUNGE_MOVE to the depth of the second peck, etc.

The following shows the sequence for drilling a 3 peck hole at (-0.688,0.500) with a plunge height of 0.200

N230 *** rapid_move X-0.6880Y0.5000Z0.2000
N240 ***first_plunge_move X-0.6880Y0.5000Z-0.1167
N250 *** retract_move X-0.6880Y0.5000Z0.0500
N260 ***first_plunge_move X-0.6880Y0.5000Z-0.2333
N270 *** retract_move X-0.6880Y0.5000Z0.0500
N280 ***first_plunge_move X-0.6880Y0.5000Z-0.3500
N290 *** retract_move X-0.6880Y0.5000Z0.2000

[kstrauss]

I hope to have rigid tapping working soon so that will make 3 or 4 users who care! On the other hand I currently use a T/C (tension/compression) tapping head with thread forming taps. Works a treat but it requires editing the Cut2D output files and I often make mistakes plus it is generally a pain.

These goodies could be easily done if Vectric were to preset variables specifying the location (they do that now), the tool number (they do that now) and depth of the feature (needs to be added) and invoke a special section of the post for each operation -- begin DRILL_CYCLE, begin TAP_CYCLE, etc.

[Leo]

Looks like you are into some pretty cool stuff. Perhaps you can get G41/G42 into Vectric as well. I like the peck drill ans will try that some day

[kstrauss]

I can easily live without cutter radius compensation. The funny restrictions on leadin/leadout are too complicated for me. Besides, it only takes a few seconds to re-post with changed tool diameter so why bother?

I'm far more interested in allowing leadin/leadout on open paths and with spiral ramps.