drilling on cylinder circumference

[merraton]

I have a problem creating drilling operation for the part you can see on the image:



There are many holes on the circumference and I don't know how to define the operations. What I managed to achieve is to define all the local coordinates for each row of holes (I assumed that if there are 36 holes on the circumference then I'll need 18 of them) and then used the tool to find holes on the given coordinates, that worked, but there must be easier way.

I assume that there has to be a function to rotate the part. Then I could define only one set of cooridnates, drill and then rotate the part for set amount of degrees, drill again and so on untill all holes are made. Any ideas?

[Brakeman Bob]

Is your post set up for B/C axis work? If it is, then all you need to do is program one hole on each row and then apply a transformation (to do that, right click one the hole job and select "Transform")

[merraton]

What do you mean by "B/C axis work"? I'm a complete newbie without any background education towards CNC

[waer]

here's a variant:


#100=36 (NUMBER OF HOLES)
#101=360/#100 (NUMBER OF DEGREES IN INDEXING)
#102=0. (METERING A AXIS)
G0 G90 X0 Y0
G43 H01 Z150.
M97 P1000
G0 A0.
X10.
M97 P1000
G0 A0.
X20.
M97 P1000
G0 A0.
X30.
M97 P1000
G0 A0.
X40.
M97 P1000
G0 A0.
G53 G49 Z0.
M30
N1000
N1
#102=#102+#101
G00 A#102
Z100.
G81 G98 Z40. R98. F100.
IF [#102LT359] GOTO 1
G00 G80 Z150.
#102=0
M99


greetings.

[Brakeman Bob]

What do you mean by "B/C axis work"? I'm a complete newbie without any background education towards CNC

A, B & C axes are the rotary axes of the machine. How do you intend to rotate your part in front of the spindle? If you machine is a horizontal mill then the chances are your rotary axis is a B (unless you have an after market 4th axis fitted in which case it be an A axis). If your machine is a vertical mill with a 4th axis then it likely that your rotary is an A axis. The C axis is when the part rotates about an axis parallel to the spindle axis.

[Aussie_CNC]

Before you define your geometry, select the little blue arrow next to the define option and select 'Around 4th Axis' (I think thats what's called from memory). You will soon find out if your post processor is not setup as the gcode will contain nothing! If you don't have the option for 4th axis geometry definition, then your post processor is setup for XYZ only and needs to be setup for XYZC (C being the wrapping rotational Axis).

[SolidCAM Profes]

Hi

Take a look at this link. It shows another option that can be used called "Multi Axis Drilling". It may help you understand this better.

Multi-Axis Drilling: SolidCAM CAD/CAM Software

Also look at this related link.

http://www.solidcam.com/solidcam-pro...-cylinder.html