Need Help!- v22 peck drilling

[68sixspeed]

Hopefully this is an easy one, I'm just learning v22 to help out with the CAM and see if we can get Bob to work or if we are going to trash can it...

first question, I got a part into mill; I seemed to get a profile to select and mill; but when I go to a drill cycle, select 'peck', it doesn't give me the options for pecking parameters? In the help, it talks about parameters being available for what I want, first peck depth, peck depths after that, clear out height, etc. Any ideas?

thanks- Dan

[69owb]

Hi If you look in the cam tree manager, right click milling tools then on part then click cutting conditions then parameters in the upper left corner. Yeah It would be nice if was more user definable in the feature Drill menu.

[68sixspeed]

thanks; it seems to do it by % in relation to dia of cutter, kind of sucks that you can't tweak it tool to tool or more importantly specify the depth of the first peck (unless I'm missing something). Interestingly the drill-peck info in the help talks about being able to adjust this, but in the help for c'bore drill, etc it references the parameter table you mentioned. thanks- Dan

[tobyaxis]

Originally Posted by 68sixspeed thanks; it seems to do it by % in relation to dia of cutter, kind of sucks that you can't tweak it tool to tool or more importantly specify the depth of the first peck (unless I'm missing something). Interestingly the drill-peck info in the help talks about being able to adjust this, but in the help for c'bore drill, etc it references the parameter table you mentioned. thanks- Dan

The reason for adjusting the drill peck this way is because of the 3-2-1 rule in drilling applications. The rule as follows is that if your drilling 3 times the diameter of a drill in depth you can go straight through. None the less you get the most amount of coolant in the first peck. Actually there are only 2 CNC Controls that I know of that will let you customize each peck. Yasnac and Seimens. They allow you to use the 3-2-1 rule for drilling. In other words 3 times the drill diameter for the first peck, 2 times the diameter for the second peck, and 1 times the diameter for each peck after. These are set with I,J, and K.

Seeing that not too many controls let you customize drill pecking it would be wise to use 100% in that setting then adjust the G-Code if you want less.

If CAM software was perfect they wouldn't allow you a separate Editor, hence Predator Editor.

N1 (DRILL .25D 118SPT COB STB)
T1M6
G90G54G40G0X-1.Y-1.S5500M3
G43Z1.H1
Z.1M8
G83Z-1.5R.1Q.25F22.<<<(Fanuc/Yasnac/Haas conrols adjust "Q" for desired peck amount)
X1.
Y-2.
X-1.
G80G0Z.1M9
Z1.M5
G91G30Z0M19
M1

[moldmker]

Check out FAQ #3 on the Bobcad website. It reviews the Cutting Conditions file.
Also remember that Bobcad has "Small" tool (less than .150" dia.) and "Large" tool parameters.

If you want an initial peck variable and you don't get one in the code, then I think you will need to alter your post processor. I think there is an Initial Peck check box in there.

Bob

[68sixspeed]

Originally Posted by moldmker Check out FAQ #3 on the Bobcad website. It reviews the Cutting Conditions file. Also remember that Bobcad has "Small" tool (less than .150" dia.) and "Large" tool parameters. If you want an initial peck variable and you don't get one in the code, then I think you will need to alter your post processor. I think there is an Initial Peck check box in there. Bob

I just went into millpostedit and looked at our post; no option for first peck depth. too bad. Mastercam is sounding better every day...

Side topic- anyone know how to get this to program G41/G42 to use cutter comp so we don't have to repost to tweak a tool size in or get a part into tolerance?

[69owb]

when you select feature profile look under patterns and then select no offset right or left. It will take some time to get the hang of it. you might want to look in to their training CD's It will give you little hints when your stumped on how to do something in the software.

[68sixspeed]

thanks!