Need Help!- Helping make CAM program for a friend...

[mcphill]

I am helping a friend with a CAM program for his Haas VF 3. At the end of this message is the start of the CAM file I made for him. The problem we are having is that the machine is going to machine home before travelling to the part home position. Can someone tell me which code to remove from the file so that it will NOT go to machine home at the start?

% O100 (PROGRAM NUMBER) (PROGRAM NAME - BLOCK2ROUGH.TXT) (POST - HAAS VF) (DATE - TUE. 05/25/2010) (TIME - 04:06PM) N01 G00 G17 G20 G40 G49 G80 G90 N02 G91 G28 Z0. N03 G91 G28 X0. Y0. (FIRST CUT - FIRST TOOL) (JOB 1 ZLEVEL ROUGH) (FEATURE Z-LEVEL ROUGH) N04 T01 M06 N05 G90 G54 X4.1482 Y-2.5066 S499 M03 N06 G43 H01 Z.1 M08 N07 G01 X3.5422 Y-2.8115 Z.0644 F2.9947 N08 X4.4355 Y-2.362 Z.012 N09 X3.5422 Y-2.8115 Z-.0404 ... rest of program runs fine...

I think he should take out the homing calls in lines N02 and N03, is that right?

[mactec54]

mcphill

Yes that is correct take that N02 & N03 out it should not be there

[mcphill]

Thanks for the fast reply! Will also edit the post...

[Donkey Hotey]

That was a safe move put into the program so an errant operator who hits Cycle Start with the spindle down near the part, won't crash into something. Why would you remove it from your post processor? How many of these parts is he going to run (in other words, how much time is really being wasted, verses screwing around with all of this)?

[mcphill]

Originally Posted by Donkey Hotey Why would you remove it from your post processor? How many of these parts is he going to run (in other words, how much time is really being wasted, verses screwing around with all of this)?

He doesn't like this move, so I will remove it for him (modify the post for him). The way he does his work is position the tool at workspace 0,0,0 and run the program from there. He is a shop owner and very experienced machinist, and somewhat "set in his ways", not an operator making 100's of identical parts...

Your comment is appreciated and warranted for "production" environments, but for this guy it is not wanted or needed.

[CNCRim]

Put Single block on...... and find out which code is doing what.

[Geof]

Originally Posted by mcphill ...... He is a shop owner and very experienced machinist, and somewhat "set in his ways", not an operator making 100's of identical parts... Your comment is appreciated and warranted for "production" environments, but for this guy it is not wanted or needed.

I also am a shop owner and very experienced machinist somewhat set in my ways; and one of the ways I am set in is to have a Z homing command right at the top of every program as Donkey Hotey suggests.

Maybe after your friend has accidently positioned the tool at the wrong location and starts a program in incremental (G91) he will decide it is best practise to pull the tool well clear of the workpiece as a first move.

[mactec54]

mcphill

If the Z was a problem then you could add were N2 was just a G0Z3.0 or what ever number he would need if he had to clear a part before a X Y move

[mactec54]

Geof

No experienced machinist is going to use a G91 at the start of a program, if they know what they are doing
You also have a T01M6 first line of code so if it needs to change the tool then it will be up already before it will make a X Y move

Now what if it does not do a tool change, well if you have just run the program you will have a Z move at the end of the program, this will place the Z in a safe place for the next start, Like G0Z3. or what ever number is safe to clear your part for the next start

[mfgbydesign]

Probably a good idea to leave the N02 G91 G28 Z0 in for a full retract prior to tool change. The X and Y in N03 are what is sending it to machine home.
Contrary to popular discussion, the G91 in N02 & N03 are NOT putting the machine into incremental mode, it refers to the distance moved (in this case "0 incremental" before moving the designated axis to the machine home position via the G28 command.

[mcphill]

Originally Posted by mfgbydesign Contrary to popular discussion, the G91 in N02 & N03 are NOT putting the machine into incremental mode, it refers to the distance moved (in this case "0 incremental" before moving the designated axis to the machine home position via the G28 command.

That part was really confusing me, thanks.

To some of the other posters, he does not use his tool crib (I have told him we need to get there, he doesn't do it yet). So, he does not need to do a tool change, as he preloads the tool before starting, and I only post the code for one tool at a time.

Slow and steady, we will get him more automated.

[Geof]

You say he is an experienced machinist yet it appears he is trying to run a CNC one tool at a time without having a clue about preparing code. That does not meet my definition of experienced.