[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]

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]

...... 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]

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.

[mcphill]

Really?

There are TONS of very highly experienced machinists out there that don't know how to spell CNC. He could run circles around most people on a manual machine before they had a CAM program done (he runs a job shop, not a production house).

He has run a shop in SoCal for 25 years, he knows what he is doing, and has tools that he knows how to use to get the job done. He could not do a 3D contour to save his life - but that is not the market he currently serves (I am helping him out along that path). He is not using the full capabilities of his equipment to maximize his investment, but that has nothing to do with being a good machinist. [/end rant].

[Matt@RFR]

Well, instead of doing all this for your friend, I think he'd be best served if you tell him to feed hold when the machine is moving in a way he doesn't want it to, look at the code, go look at his G/M code list and figure it out. He's never going to learn if you hold his hand like you're doing.

[MrWild]

For the sake of discussion I too am a very experienced T&D with manual machines. I was asked to make some small widgets on my new CNC mill and went through the process of writing a program, then making a part fixture, and running the parts. Another shop owner was going through my work and asked why I had quoted so high for the parts. I explained the fixture and all to his listening and helpful ears. When I got done, he said he'd have made all the parts in one bar with extra stock on the bottom. Once the parts were made and still attached to the bar, he'd have flipped the bar over and machined the bottom off and parts to size. Needless to say, I listened and learned quite a bit by not having an attitude. Just because I was hot spinning cranks, didn't mean I was hot with CNC. There are tricks with CNC a manual oriented person wouldn't normally think to use.

[mcphill]

mactec54, thanks for your prompt and spot on reply, confirming my suspicion.

To all those with "constructive" criticism, thanks for that too, but enough is enough. I got the confirmation I needed, my friend and I have learned a few things, are happy with the outcome, and have moved on.

I am moving on from this thread, and don't plan to be back. As much as I understand what some of you are trying to preach, I know the limits and speed with which I can help my friend along. We have made SO much progress on the past month alone (far more than the last 4 years, as I now have a knowledge base in CAM that I did not have a year ago).

[double a-ron]

Mcphill, for a long time I've had an embarrassing secret I never told anyone. If it wasn't for reading your post I don't think I'd have the courage to admit this now, I can't spell cnc either.

While this may not be an issue to say, a bus driver or a gynecologist, you can see how this would effect the self confidence of a cnc programmer. Imagine filling out a loan application and everything is going great until you get to the occupation box. What do you do? You can't just put programmer, because inevitably the loan officer is going to say something like "computer programmer! I was going to go to school for computers". And he'll go on and on rambling incoherently about this for hours, and just when you can't stand it any more you'll say "CNC programmer" At this point he's been blathering on so long that he has no idea what your talking about. So you say "cnc programmer, I ah, program cnc machines not computers". So now you got this guy sitting there and you know he's thinking why didn't he just write down cnc programmer. If he only knew...

I've been living with this dirty secret for a long time and I just want to thank you for helping me get that off my chest. Moving forward I plan to learn to not only spell cnc, but write it as well. I know this will be a long and difficult journey, but I'll know I'll get through it.

I know there are other who have this same problem. Come forward and share your experiences. Only through sharing will we be able to overcome this obstacle.

[Donkey Hotey]

The way he does his work is position the tool at workspace 0,0,0 and run the program from there.

This is the part all of us must have missed. These guys aren't using any work offsets. They dial the tool to where the part is (give or take a sliver of cigarette paper), then punch the green button.

Wow! Good gawd, somebody show that poor guy how to set work offsets and actually use his machine.

[Geof]

This is the part all of us must have missed. These guys aren't using any work offsets.....

They must be using them; the program calls for G90 G54 and G43 H01 on lines N05 and N06.

The only way to position the tool at 0, 0, 0, and then run a program from there is to write it completely in incremental.

[Donkey Hotey]

OK, you got me. Now I really can't figure out what was wrong with the safe move.

If he's a job shop and running one or two parts at a time, that safe move wasted 10 seconds of his life. If he was running 100 parts, he'd save 16 minutes over the run. If he's making two parts, he saved 20 seconds. It took longer to ask the question.

I wouldn't bother editing out the lines (even knowing they're in there) for only 1-2 parts. Somebody is picking the flypoop out of the pepper.