Machining time in NC file?

[Samvatas]

Hi guys!

I want to get machining time (shown in backplot) in my post to output it at the start of NC file.

Actually, I'd like to get it for the each tool in my program (to output it in the ptooltable section), but any advice would be appreciated.

Any Ideas? Is it possible at all?

I found only 15105 parameter in MCAMX5_NCI_Parameter_Ref.pdf (but I'm not sure because it's always equal to zero). What's this parameter for?

Thanks.

[K2csq7]

I tried that maybe a month ago...

I found only 15105 parameter in MCAMX5_NCI_Parameter_Ref.pdf (but I'm not sure because it's always equal to zero)

 

Same thing here???? always zero???

[Samvatas]

Yes, I checked it couple of times and it was always zero.

I thought if Mastercam had so many parameters it must had such parameters for machining time (hours, minutes and seconds enough).

May be such parameters are not implemented yet (and 15105 parameter is just a dummy). Or may be they even ain't planned to implement. Who knows.

Anyway, I couldn't figured out what's the parameter for. MCAMX5_NCI_Parameter_Ref says something about "Calculated cycle time for NCI section", but who must calculate the time - post or me, and why it's always zero?

[Superman]

Have you looked at the mill.set ?

and how this setup sheet handles time, limits etc

 

It would be a good place to start

[Samvatas]

Thanks for good advice! I looked at it and found a couple of bugs

For instance, here is the ptime section:

ptime #Distance calculations

dx = x$ - prv_x$

dy = y$ - prv_y$

dz = z$ - prv_z$

len = sqrt(dx^2 + dy^2 + dz^2)

if gcode$ = zero, ptimer #RAPID time and length calc

if gcode$ = one, ptimel #FEED time and length calc

!x$, !y$, !z$, !fr_pos$ #Update previous [prv_?] variables

if fr_limits, pfrcheck #Track MAX/MIN Feedrates if requested

What about arc motions? Shouldn't they be calculated as well as linear and rapid motions?

Nevertheless it's a good start indeed. Thanks again!

When I fix it (or if I fix it ) I'm gonna post here the result for other people.

P.S. It's a pity that Mastercam doesn't have operation's parameters for backplotted time - it would be easier to output it at the top of NC file.

[Allan]

In the set-up sheet .set file the arcs are linerized (look for linarc$) that way all the moves are linear, and the ptime postblock works just fine.

[Bryan Johnson]

In the set-up sheet .set file the arcs are linerized

 

Would that be a problem if someone wanted to use the ptime method in a machine post?

[Paul Decelles]

Cycle times need to be calculated based upon the distance traveled and the speed at which those distances are traveled. Mill.set linearizes arcs and forces long hand dill cycle output to break the motion into rapid and linear motion which can in turn be calculated for time estimates. It is not possible to do this while you are actively post processing a file for output. The best I could suggest would be to use a the ppost$ postblock to reprocess the NCI file using some kind of stripped down .set file and then to merge the results in to the NC file previously generated by the pst file (not for the faint at heart).

[K2csq7]

Thanks for the info Paul, greatly appreciate your time.

Could you explain what param 15105 is? In the param ref doc. it says something about backplot time...

[Jimmy Wakeford from Barefoot CNC]

You could find the length of the arc with something like this:

 

#HomeMade variables
arc_ratio : 0
arc_length : 0

pfind_arc_length        #Find arc_length by using sweep angle and radius
    arc_ratio = abs(sweep$) / 360                         # Find ratio from sweep angle / 360
    arc_length = ((arcrad$ * 2) * 3.14159)) * arc_ratio   # Find circumference of total cirlce then multiply by arc_ratio to get length

 

I think this will work (as long as I got my variables right )

 

Once you have the length you could add a ptimea post block for gcode$ = 2 or gcode$ = 3

[Samvatas]

Does anybody know why rapid length in the set-up sheet differs from the one in the backplot window (in most cases)?

[nor draw]

hi, listen i am a new guy so this may not help but we use a excel file to change tools amoung machines,\it is on lathes

but say a cnmg on 3101 is diffent than 3104 the mastercam is programmed to a cnmg then the sheet takes over and corrects it for both machines.

[André Lapointe@In-House Soluti]

Paul is right, doing this while posting is a pain, I had to do this once and it was not as easy as it looked like at the beginning!

 

It was for tool life management along with a cell management system. Not only is it a pain to calculate it right, but to have it at the beginning of the NC it means that you need to output the G codes into a sub file while you calculate the time based on each moves and then at the end you need to bring everything back into the main NC file to have the time at the beginning instead of the end of the file. Also you need to find a way to store each tool time separatly and to add to each of them if the tool is re-used later in the program.