Problem- NL2500 with CAPPS

[Bobesmo]

We have a new NL2500 W/ CAPPS Programming and I am trying to muttle my way thru it....How do you make a drill retrac in a pecking cycle,(come all the way out of part) at a preset amount?

[underthetire]

Search the manual in the control. Works good since its in PDF. Help button, select the manual you want. I don't have the lathe manual here.

[fordav11]

do you want to know in CAPS or with standard G-code? also bear in mind CAPS cant do everything, some of it needs minor manual tweaks.

[fordav11]

The exact screens and programming sequence will depend on which version CAPS you have.
Here's a few pics from my CAPS......

On the drill page (1st pic) you can set the depth and other simple things.

If you press DETAIL you will get more options to adjust (2nd pic).
'CENTRING' means it feeds slower (lower by 20%) until the drill is cutting at full diameter then it feeds at normal feed rate.
'CUT DPTH' means it feeds this far in peck accumulations then retracts to the start position 'START Z' plus clearance.
'IN FEED' & 'OUT FEED' is the feed rate applied to the peck clearance pullout and the feed after the tool rapids back down the hole as it feeds back into the material.

If you press 'TOOL COND.' (3rd pic) it will allow you to change T code, speed, feed and peck amount which is shown as 'STEP AMT'.

In this example the drill will....

1. rapid to Z3.0 then X0 (3 is nominal drill Z clearance set in CAPS parameters)
2. take 5mm pecks with a small back-off until 50mm is accumulated (Z-47.0)
3. rapid to Z3.0 then rapid back down to where it previously stopped less clearance (Z-46.0.... 1mm less set in CAPS parameters)
4. continue taking 5mm pecks until 97mm depth is reached (47+50)
5. rapid to Z3.0 then rapid back down to where it previously stopped less clearance (Z-96.0)
6. continue taking 5mm pecks until 147mm depth is reached (97+50)
7. rapid to Z3.0 then rapid back down to where it previously stopped less clearance (Z-146.0)
8. take the last peck to 150mm full depth
9. rapid to Z3.0 then X300.0, cancel tool offset etc etc.

if you need more tool control than this you will have to program it manually with G-code.