Eliminate the A0. from the G28 line.
Mike
I need to get the tombstone to turn 90' and then stay there till I can drill, countersink, and tap with it in that position.
I managed to get the tombstone to turn with a A90, and drill. But when it gets through with that drill and goes to get the next tool the G28 makes it go back to 0.
There has to be a way to get it to stay till I tell it A0.?
Similar Threads:
Dennis
Eliminate the A0. from the G28 line.
Mike
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
Is it the tool change program that makes the G28 ?
When you program M6 ?
Oh I forgot to mention, there is no A0 or any A codes in my post at all.
I have to place the A codes in manually. This old Teksoft dont do it for me.
So what I did was put the A90 in the line with the G57 and that was all.
I assumed it would stay at that position till I put A0 and the end of my program.
Dennis
Yea, I will definitely make sure the tombstone is back first.
Oh something I just thought of too. Teksoft always puts a Z0 at the end of each op and boy that is a disaster on a EC400.
Feeds the tombstone into the spindle!
Dennis
I am about halfway afraid to remove the G28 because at this point it is whats parking the tombstone before a tool change.
Unless there is a code specific for parking it.
Dennis
All you have to do is run it a 5% rapid and watch it with your hand on the emergency button.
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
As haastec said, post some of your code here.
Mike
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
I have always prefered G53 Z0. Or G53 X-15. Y0 Z0 for a vertical mill that puts it closest to the operator in Y, and centered in X, and Z home. You can very easily put it anywhere you like.
Here is how my posts typically end before the next tool. And that Z0 you see in there sends the work into the spindle. So I always delete it. For some reason on this EC400 the Z0 is not send to home.
N65 X15.902
N70 X18.264
N75 G80 G00 Z5.
N80 G54 G90 X18.264 Y-.75
N85 G49 G28 Z0 M09
N90 M01
N95 (90' C.SINK)
N100 T09 M06
N105 S800 M03
Dennis
The reason is that G49 cancels the length offset but not the work offset, so it tries to drive the face of the spindle to your G54 Z0 position.
Fix your post pronto, because this will bite you in the a$$ sooner or later and it will not be pretty.
If you just replace your G49 with G91, that combination of code will send Z axis to the home position. The combination of code is key!
I am not trying to insult you with this question, but what is your experience level with G-Code programming? I know you are using Tek Soft, but how well do you understand the code it is producing?