[mousongie]

Hello Mates!

Im doing drilling and tapping operation on some hubs. Hover for the benefit of productivity,i would like to machine 3 (three) parts at a time , whereby i will drill and tap the first one (G54), going to the second part(G57), do the same, and then, the last one (G58).

I would like to know how to set EDGECAM so that the NC file output , corresponds with the idea explained.

Thank you in advance,

[jtreanor]

Hi Mousongie,

Edgecam menu - Geometry - Create CPL
create two new CPL's (G57 & G58)

If the parts are identical, you can create the new CPLs in the
exact same location as the first G54 (top) CPL

complete all instructions for the first part,
from the menu select - Move - Index to the G57 CPL
note - you must type 57 in the "Work Datum Override" field otherwise
Edgecam will automatically assign the next available number (55)

now just copy all the drill tap instructions after the Index

repeat for G58 - you must type 58 in the "Work Datum Override" field

***********

To minimize toolchanges use Rationalize By Tool

[tummen]

We are using Heidenhain TNC so we dont use G54 and so on but we have the same kind of problems as you.
There are some ways to make this work.
You can index to G57 and then use Edit-Transform-Repeat to copy the instruction results without having to duplicate instructions (no risk of having changes forgotten on one location on the tomb)
There is a, more and less, good solution
this is Edit-Matrix mode-start + end. as long as you don´t use operations(for me it has always messed up the oplist after having operations in the instruction list)
Good is that it handles all logic to reuse the tools on all locations before jumping to the next tool.
Bad is that it only accepts incremental moves to the next tomb location (no index change to G57) a solution is to use code in the post processor to detect that indexing x+1000 means jumping to G55+(increment/1000) but we saw this solution as to easy to make mistakes in the long run.

The solution we now use is one that I created outside the control of edgecam

when i press post i get a question from my postprocessor if i want to get multipreset och simple posting.

if i make a multipreset the post processor:
puts some Q vars in the start of the program to hold first index (G55)
and how many to use 3 => G55+G56+G57

puts a lable start before each toolcall and closes any old subprograms. I also count the number of toolcalls i have and store in a Q variable. all Lables are numbered is such a way that they don´t collide with normal labling in edgecam output.

in the end of the program a loop is inserted that i jump to from the beginning of the code.
I need to know the number of toolcalls so i can´t put this loop in the top section.

i then
Qlable = first lable no.
do
Gindex=first
do
set index
lift tool to safe Z level
call lable to do milling for tool 1
Qindex=next
LOOP while index < count
next
Qlable = next lable no.
LOOP while lable < count

i also added a Q value for Z abs level for retracting before moving to next index

this solution has been tested now for a month on about 5 programs and it works really good for us.

[jtreanor]

Hi Mousongie,
Is this a vertical mill or horizontal with 4th axis tombstone ??

[mousongie]

Hello guys, thanks so ever for your input. I really found them very helpful.

[mousongie]

Hello jtreanor, how are you my friend? Thanks a lot for your help. Well, the machine is a 3axis vertical mill.