What Am I Doing Wrong?

[partsman]

I have ran this program several times and never encountered a problem. I just received a new Mari Tool Rougher so I added a roughing operation to test it out. Now, when simulating in graphics mode, the final chamfer operation is shifted down a couple inches. I just can't see the problem in the code. Any suggestions?

Maybe this a problem in graphics mode only? I really dont want to waste a block of material just to try it though.


Any help would be appreciated.

[Machineit]

I have ran this program several times and never encountered a problem. I just received a new Mari Tool Rougher so I added a roughing operation to test it out. Now, when simulating in graphics mode, the final chamfer operation is shifted down a couple inches. I just can't see the problem in the code. Any suggestions?

Maybe this a problem in graphics mode only? I really dont want to waste a block of material just to try it though.


Any help would be appreciated.

I ran it in my simulator and saw nothing wrong. I would check the offset of the offending tool. Did you set the tool when you had a clearance set in the G54 Z offset? For example. did you have a 2" clearance entered in the G54 Z offset and then set the tool? Can't do that.

Secondly, I do not like you style of code writing at all. You never clear your tools prior to a tool change and you go down and to the XY location in the same move. That is just asking for trouble. Move to your XY location then go with a G43 line to bring to tool to the clearance plane. Like: G43 Z.2 H02 M08. You are just asking for trouble with G43 H02 M08, G00 X2. Y2. Z.2 or something like that.

Lastly, even though you may not technically need it, you should put a " G91 G28 Z0" and an M05 prior to just calling a tool change.

Mike

[partsman]

Thanks for the reply Machineit!

It must just be a problem with the graphics page because I decided to just run it (slowly) and see what happens. It cut just fine.

The code just comes from OneCnc. I'm still really new at this and I have not really had time to try to fine tune any of the settings.... or really find out WHAT I should be tuning to be honest. I guess the x,y,z moves would be a potential collision problem? Is that why you should avoid those moves?

What does the G91 G28 Z0" and an M05 do?

[Geof]

M05 turns the spindle off.

G91 G28 Z0. is a hokey way of sending the Z axis home. At least in my opinion it is hokey. G28 is the command to home the machine via a reference point. (Read your manual it says something like that.)

With the command G28 Z0. the machine first moves to Z zero in the active tool offset/work offset system, then moves to the home position.

When the incremental command G91 is added making it G91 G28 Z0. the machine does an incremental move of zero (in other words it doesn't move) then it goes to the home position.

And you have to remember to follow that command with a G90 to put the machine back into absolute mode.

Use G53 Z0. and the machine moves straight to the home position. G53 is the command to use the machine coordinate system.

[Machineit]

Thanks for the reply Machineit!

It must just be a problem with the graphics page because I decided to just run it (slowly) and see what happens. It cut just fine.

The code just comes from OneCnc. I'm still really new at this and I have not really had time to try to fine tune any of the settings.... or really find out WHAT I should be tuning to be honest. I guess the x,y,z moves would be a potential collision problem? Is that why you should avoid those moves?

What does the G91 G28 Z0" and an M05 do?

You are posting in the Haas forum, what machine are you running? That post is a big problem, you need to get it fixed.

When you go to a location in a G00 move, all axis's move at a rapid speed and with no regard to clearances. What ever axis gets there first is not controlled. So if you are going from one side of the table to the other and it's 12 inches or so, your Z axis will most likely get down before your X axis gets to the proper location. This could have disastrous consistence's. Always go to your next location before bringing the next tool down.

For example:

T1M06(.220 DRILL)
G90G54X-2.5938Y4.4925S4000M03
G43H01Z0.1M08


Also end each tool by moving it to the tool change position. Don't just call a tool change. Yes, a tool change will stop the spindle and turn off the coolant, but the coolant will come right back on after the tool change and not shut off until it is actually make the tool change and will put coolant into the changer. Turn off the coolant and the spindle prior to the change.

Example:

G00Z1.M09
M05
G00G91G28Z0.


If that is a OneCNC post, it is not good. Check with them for one specifically for the Haas or whatever machine you have.

Mike

P.S.: Get a book of G and M code and learn what they are. You should be able to watch the screen as it runs and know exactly what each code is going to do for the machine.

M

[partsman]

The machine is a VF2. The code is straight from the stock OneCnc post for the HAAS. There is a second HAAS post listed but I have not been able to get it to work correctly at all. I will email them & see if there is a newer one.

Also end each tool by moving it to the tool change position. Don't just call a tool change. Yes, a tool change will stop the spindle and turn off the coolant, but the coolant will come right back on after the tool change and not shut off until it is actually make the tool change and will put coolant into the changer. Turn off the coolant and the spindle prior to the change.

Makes sense.

P.S.: Get a book of G and M code and learn what they are. You should be able to watch the screen as it runs and know exactly what each code is going to do for the machine

I guess I knew what the actual G codes did but was not sure of the reasoning for using them in the way that you posted.

[Machineit]

M05 turns the spindle off.

G91 G28 Z0. is a hokey way of sending the Z axis home. At least in my opinion it is hokey. G28 is the command to home the machine via a reference point. (Read your manual it says something like that.)

With the command G28 Z0. the machine first moves to Z zero in the active tool offset/work offset system, then moves to the home position.

When the incremental command G91 is added making it G91 G28 Z0. the machine does an incremental move of zero (in other words it doesn't move) then it goes to the home position.

And you have to remember to follow that command with a G90 to put the machine back into absolute mode.

Use G53 Z0. and the machine moves straight to the home position. G53 is the command to use the machine coordinate system.

No offense meant Geof, but G91 G28 (XYZA etc) is the way every post I have ever seen is written and the way Haas programs for demos in their manuals. I think I would have him stick with that for now.

Mike

[underthetire]

G91g28 z0 is pretty much industry standard. The only way it doesn't work right is if you forget the g91 with it. We use the g28 command on all our haas's and all the fanuc machines. It's what it's there for.

[Geof]

No offense meant Geof, but G91 G28 (XYZA etc) is the way every post I have ever seen is written and the way Haas programs for demos in their manuals. I think I would have him stick with that for now.

Mike

Yeah I know.

I just think it is ridiculous that in absolute G28 commands the axis to first go to the reference point then go home. It should go straight home from wherever it is. At least Haas does make a good job of using G28 because if no axis is specified the Z goes home first followed by the others so at least you don't wipe across the table.

[Ydna]

That's actually why we don't teach G28 it school. For the people that understand the movements everything is good, but for those that don't...well stuff can go really wrong if you're not aware of what will happen (lol)

[Geof]

...well stuff can go really wrong if you're not aware of what will happen (lol)

Like shearing off a 3/4" carbide mill just below the holder in the first few days of programming and running my VF0.

[Machineit]

Like shearing off a 3/4" carbide mill just below the holder in the first few days of programming and running my VF0.

Yeah, learning can be expensive, but sometimes those are the lessons that really TAKE!

At least the way most are taught and the way most posts are written, Z is always taken home first followed by any other axis such as Y. Normally between tools only Z is homed anyway.

If I were teaching now, I would still teach the G91 G28.

Mike