Single step steps more than one line....
when I use single step to validate a program EMC2 makes always a couple of lines, how can I change that situation? When I programmed code for prototypes which are sometimes out of very expensive materials I use the single step in combination with the feed overdrive: feed overdrive to zero and then the next step, then I increase the speed to show how everything works... Ok! then Feed overdrive to zero and the next step..... but EMC2 goes through more than one line in single step mode! It is a bad situation!
hope there exists a simple solution! Ingo
Please Log in or Create an account to join the conversation.
What happens if you hold the single step button down? (not with one of your expensive parts in place)
Please Log in or Create an account to join the conversation.
Please Log in or Create an account to join the conversation.
this is a "normal" behaivour of emc (the interpreter) The single step mode is useless for professional applications cause you will never know how many lines will be executed and wich line will be next.
regards, Thomas
Please Log in or Create an account to join the conversation.
That was using the onscreen button. Are you doing it some other way? (There is a halui pin that could be wired to a hardware button for example)
I only have 2.5~pre working on my computer though
Please Log in or Create an account to join the conversation.
you have to press 3 times the button until you get a highlighted line in the listbox of axis and the machine begins to move.
This is a bad behaivour cause you will never know WHEN the machine starts to move.
If you press the step button 8 times the program reaches line 12 of the nc-code. Next press jumps to line 18 of the nc-code. User expected line 13.
regards. Thomas
Edit: Think this is caused by the settings of the path mode...
Please Log in or Create an account to join the conversation.
This seems to be an issue with the line highlighting, I think that program execution proceeds one line at a time, for example the spindle starts on click 6, which is line 10 (which is correct, allowing for the 4 comment lines at the beginning) even thought the highlight is still on the M6 line. The next click causes line 11 to execute, and moves the highlight there. This is a single program step (good) but a triple line highlight jump (bad).Well, open the 3dchips.ngc and step thru the program...
you have to press 3 times the button until you get a highlighted line in the listbox of axis and the machine begins to move.
If you press the step button 8 times the program reaches line 12 of the nc-code. Next press jumps to line 18 of the nc-code. User expected line 13.
Edit: Think this is caused by the settings of the path mode...
Indeed, it does seem to be the G64P0.1 blending. If you program G61.1 (exact stop mode) then the behaviour is different.
What I think this means is that the interpreter treats moves within the G64 tolerance as a single blended move, and single-steps through them as a single move too.
I can see an argument that this is the correct behaviour, and also an argument that it is not the expected behaviour.
Line-highlighting on non-motion lines does seem like a bit of a bug though. If that was fixed the single-step would be rather more intuitive.
Please Log in or Create an account to join the conversation.
this behavior is very bad when you are milling very expensive parts.... I have sometimes parts on the machine (which I'am now fitting with EMC2) which costs about 50.000 $ so there should't be any mistake!!! For that I'am often went through the program in single step always reduced the speed to zero, when I start the next step I increase the speed slowly that I can see what happen, when everything is OK I increase to full speed till the next line... To fix this bug EMC2 should swich to G61.1 while stepping over and swich back when the program run normally. For information: Controllers like Siemens, Haidenhain, Fanuc, Phillips.... step always one line to the next one, also lines like N20 G90 or N30 S2500, that are all lines for the single step
Please Log in or Create an account to join the conversation.
Imagine if you made the mistake of putting G64P100 instead of G64P.100 and the control system changed your G64 mistake to G61 for single step. You would not see the mistake when your milling your machinable wax one step at a time but only when you are in auto machining your $50,000 part.
John
Please Log in or Create an account to join the conversation.
yes you are right, my machines have no possibility to set the accurancy of G64 so they have an other algorithm... Ingo
Please Log in or Create an account to join the conversation.