deep drilling

[Tcommis]

I need to drill a series of .093 holes 4" dp. I want to drill 1.5" with a jobber length drill then follow with a long drill. Is there a way to start the second drill at 1.5" dp. yet retract out of the hole to pull the chips?

[Guest CNC Apps Guy 1]

Ok, Assuming that the bottom of the part is Z0;

 

Create a point(s) at Z2.5. Toolpaths, Drill, select the point. Set the TOS at 4. Absolute and the retract at 4.1(or whatever you want for where you want it to start feeding. Now create a point at Z0 (which is 4" from the top of the part using my method). Toolpaths, Drill, select the bottom point(s). TOS is Z2.5 Abs. Retract is 2.6 Abs. Clearance set for anything over 4". UNCHECK use clearance only at the start and end of operation.

 

HTH

[Tcommis]

James--

don't see the box you said to uncheck. using v8.1. using clearance drill wants to feed from top of part.

[Guest CNC Apps Guy 1]

Good reason you don't see that check box. You're running 8.1, it's only in 9.x

 

Retract needs to be your safety distance from the previous depth and clearance needs to be above the part.

[Tcommis]

yes, i have that set but i need to pull the drill out of the hole after every peck for chip evacuation without redrilling initial 1.5"

[MACHINEMASTERG]

some controllers have an option for added clearnce above the r plane i know our haas has this ....i use it in the same situation you have ....what controller do you have

[EX-wccprogrammer]

If I understand your question correctly, you will need to customize your post to deal with this type of drilling operation. Standard drill cycles will only retract to the r-plane until full depth is reached, then retract to the clearance plane.

 

I ran into a situation similar to this, only I was peck drilling using a 90 degree head. I ended up writing a macro to deal with the cycle.

[Tcommis]

I am using an old fadal cnc88. I know ugghhhh.old version of MC as well. all is working against me!!

[MACHINEMASTERG]

write it up in a long hand drilling sub rotine the way you want it and call the sub at each hole ...??????

[Guest CNC Apps Guy 1]

Ahhhhhh, I see said the blindman to his three deaf children. You'll need a custom drill cycle I believe since you ned your retract to come out of the part....

 

Hmmmmm. I'd pput in a call to Fadal Applications Engineers in Chatsworth and see iof they have some variables you can plug into the canned cycle to get that.

 

Your next best option would be to do a hole long hand, edit the retract and sub it.

 

HTH

 

 

Sorry

[EX-wccprogrammer]

No problem...

 

Here is what I would do....

 

Write the peck cycle you want as a sub program using G00 and G01 commands. Then call that sub at each hole location.

[EX-wccprogrammer]

James, you type faster than I do...

[Guest CNC Apps Guy 1]

... and Greg types afaster than both of us!

 

[Tcommis]

those sound like great ideas guys. thanks for all your input

[P_Scott]

Tcommis,

 

You could also call us here and ask for post modification help from Steve. He's the post guru. I've never seen anything he couldn't do with the post processors. HTH

[Rick McAllister]

Tcommis,

 

How about a deep hole macro. That's what we use here. Have a drill cycle set up to post out the required variables. SWEEET.

 

I wish I could share it with the forum but it's company property.

[David Czerw Triumph Gear Systems]

Maybe "X" will have that in its drill program. I sure could use it

[Tcommis]

a deep hole macro would be great. if i knew how to write one it would be even better. it would be a nice option.

[Camdude®]

Version 9 also includes the custom drill parameters page to set up non-standard drill cycles. i just used it the pother day to set up a custom cycle for a gun drill application. this application is also avalaible in version 8. you must tweak post to use variables but it works nicely. HTH

[Glenn Stephens. from CCCS]

I think the easiest way to deal with this would be to write the toolpath as if you're peck drilling all the way down, then set "usecannedpeck" in the post to "no" (this gives you longhand), then hand edit out the G0, G1's in the .NC file that end up cutting air.

[Surface]

Thats the way I would do it as well. I don't imagine you want to rapid into the hole anyway. Another sugestion is to not retract the dill all the way out of the hole. With such a long drill, I think you may have some run-out.

[Thad]

You can tweak a post all you want or create a custom drill cycle, but if the control doesn't support it, it won't work. Can anyone confirm or deny this?

 

Thad