Slow drilling

[CosmosK]

I did some peck optimization for a whole bunch of deep hole I had to drill.

I made a program drilling each hole 1mm deep, the copied the code into excel. Using formulas and the like in excel, I got to where I could duplicate the routine easily. It was some work, but seemed to pay off. It wasn't very complicated, as the peck depths were the same, basically just changing XY and repeating the routine. You really notice how much time you're wasting when drilling a bunch of holes with all those unnecessary feed rate moves.


video:

[Adrian]

Do you have RAPID_PLUNGE_TO_STARTZ = “YES” in your Post Processor?

http://forum.vectric.com/viewtopic.php?f=18&t=22636

[kstrauss]

Yes, I added that option immediately after the previous exchange on this topic. It does "retract to the previous cut depth rather than safe height" as is shown in my previously included output snippet. The problem is that "cut depth" is the depth of the start of the cut rather than the depth of the end of the previous peck.

[CosmosK]

the problem with retracting to previous cut depth is chip removal, i.e. it doesn't work so well.

[CosmosK]

Do you have RAPID_PLUNGE_TO_STARTZ = “YES” in your Post Processor?

http://forum.vectric.com/viewtopic.php?f=18&t=22636

Does this only affect drilling? Thanks!

[Adrian]

No, it makes all plunges from the Z1 to the Z2 height become rapid moves rather than plunge rate moves. It doesn't change anything from the Z2 downwards though.

[kstrauss]

the problem with retracting to previous cut depth is chip removal, i.e. it doesn't work so well.

Correct. That is why I'd like to retract to top of stock, plunge rapid to depth of last peck, peck and repeat. Unfortunately, the "plunge rapid to depth of last peck" is a "plunge slowly (feed rate move) to depth of last peck". This takes forever when drilling many deep (many pecks) holes.

[scottp55]

Just curious what material you're drilling?
scott

[CosmosK]

the problem with retracting to previous cut depth is chip removal, i.e. it doesn't work so well.

Correct. That is why I'd like to retract to top of stock, plunge rapid to depth of last peck, peck and repeat. Unfortunately, the "plunge rapid to depth of last peck" is a "plunge slowly (feed rate move) to depth of last peck". This takes forever when drilling many deep (many pecks) holes.

It's not all that hard to do in excel. I can send you my file if you'd like (info@cosmos-industrial.com). I should make it all fancy with macros... one of these rainy days. I drilled out my 1.5" 7050 AL table with a pattern of 4.2mm holes. I think it ended up being 160 or so holes. It saved a bunch of time.

[kstrauss]

In reply to scottp55:
My use of Cut2D is for simple jobs on a Tormach 770. Rapids are at up to 135ipm so slower than some routers but much faster than feed rates for drilling.I am usually drilling aluminum with some parts of Delrin(R) (acetal) or other plastics. Occasional work is with various steel and stainless alloys such as 303, 316, 12L14, 1144 and 4140. Parts often have dozens of deep drilled holes so the time wasted with slow feeds is significant. Since most of my parts are prototypes or very limited production, editing the Gcode for each is not reasonable.

[kstrauss]

the problem with retracting to previous cut depth is chip removal, i.e. it doesn't work so well.

Correct. That is why I'd like to retract to top of stock, plunge rapid to depth of last peck, peck and repeat. Unfortunately, the "plunge rapid to depth of last peck" is a "plunge slowly (feed rate move) to depth of last peck". This takes forever when drilling many deep (many pecks) holes.

It's not all that hard to do in excel. I can send you my file if you'd like (info@cosmos-industrial.com). I should make it all fancy with macros... one of these rainy days. I drilled out my 1.5" 7050 AL table with a pattern of 4.2mm holes. I think it ended up being 160 or so holes. It saved a bunch of time.

Thanks for the offer but as I believe that I mentioned in another post most of my work is with one-off prototypes so extensive postprocessing of Gcode is not really warranted. That said, I have used Excel to generate the Gcode to do 3D profiling of fancy shapes generated by probing an object and applying various equations to the measured surface.

[Leo]

You could make "one" incremental drilling pattern and make it into a sub program, ending with m99.

All you would need to do is add a M98P__ at each hole location.

[kstrauss]

Yes, assuming that all holes are the same depth. What is really needed is the ability to define a procedure for drilling/tapping that has named parameters for feature depth, start depth, etc.

[scottp55]

Thank you.
scott

[CosmosK]

Well, I made a macro to optimize peck drilling. If anyone wants a copy, send me an email (info@cosmos-industrial.com). I'd post it but I'd like to know where it goes in case I find a bug so I can alert people (EDIT: like forgot a Z on the first line). Use at your own risk of course.

I added a buffer, so when it rapids down to the previous drill depth, it can stop just shy to account for machine deflection. To use, just copy in the x,y locations and set the parameters on the left, then click run.