[luckyyyyyy]

hi every one...

please help me about this matter...

actually you know about Gcode...

so after generating Gcode from masterCAM...

I found following lines at the end of Gcode..

--------------------------
N9 G91 G28 Z0.
N10 G28 X0. Y0. A0.
N11 M30
%
--------------------------

this means that after the operation is completed the tool move to refrence point " 0,0,0 " ..My problem is that I dont wana tool move back to reference point...I want to keep tool at that position...

actually every time during machining the tool move back to refernce point(zero point)... i think these should be one option in masterCAM for the keep tool at last machining point...please tell me how can i solve this problm..

one think ...what do you think is that masterCAM problm or Post Processor ...?????????


please help me and reply me fast...thanks...

[Superman]

This series of code that mastercam outputs is a generic " put things back the way you found them" senario

It all depends on the machine and control, does you machine know it's position at boot-up or do you have to home the axes

Some machines set the "part origin" from it's current homed position. If you are not at home, how is the machine capable of setting the work datums. If you left the code "as is", what do you hope to gain--- 1/2 a second of cycle time, and 1 hour of setup grief, or do you leave it alone.

Tool change is usually at a pre-defined point, either home in Z or at a known point. Mastercam would be using a "SAFE POINT" for all the above, and it would be up to the programmer or operator to "chop" the program to gain any time for a production type job.
Single or low quantity type jobs would not be worth the effort to trim time out of it, as it would take 1/2 hour of editing to save 5 minutes of time- so it's not really worth going that direction.

Even keeping tool retracts short as possible, is not cost effective. You run the danger of a descent crunch ( the tool and or the part will end up in the
skip ). Yes, keep the retacts respectable ( say 3mm or 0.1" above the highest point )

[CNC TECH]

It sounds like your Post that is causing your problem I'm not well up on the parameters the mastercam posts use but if you want to mail it to me i'll take a look and hopefuly mail you back a new post with this movement eliminated.

the previous post is very correct about avoiding a crash but I think I could give you 2 new posts to try the first to eliminate the movement to 0,0,0 after tool change and one to eliminate the movement completly just a Z,0 to move your tool from the job safely

[luckyyyyyy]

Thanks alot for advicing...

actually I wana solve this matter...please if you have solution what I want then kindly tell me...I just want to keep tool at last position ...dont wana back to zero point(reference point).....so kindly tell from where can I set this command(from MCX or Control Definition or Machine Definition) from where????????????????


Its sure that these two following lines are auto generated by masterCAM...but I dont want these ...how can I control these...?????????

N9 G91 G28 Z0.
N10 G28 X0. Y0. A0.



thanks...

[rockchopper]

Are you using MPFAN.PST? Below is the part of the post you need to modify. Put a # in front of the red line. After this the line will be ignored. If you don't know how to edit the post. Don't do it. This however will not eliminate N9 G91 G28 Z0. I wouldn't take that part out anyway.


peof$ #End of file for non-zero tool
pretract
comment$
#Remove pound character to output first tool with staged tools
#if stagetool = one, pbld, n, *first_tool, e
pbld, n$, *sg28ref, "X0" "Y0." "A0", protretinc, e$
n$, "M30", e$
mergesub$
clearsub$
mergeaux$
clearaux$
"%", e$

[CNC TECH]

Luckyyyyyy Its not that I want to hide what I would do, I would give you explanation of how to do it yourself, it's just I need to workout where the line is being generated and I'm not sure how mastercam works it could be in parameters for machining within the program or it comes from the post.

I will see if i can find a demo version of mastercam and look for you but i dont think a demo version will have a post with it thats why i asked to see your post, send it privatley to me.

[PROFCNC]

Hi all,
Here is one thing to keep in mind. Altering or editing the post may not be a safe option long term. It is best to understand how you may be able to edit the program after posting to tailor it. The sequence line N9 is the safest way to send a spindle home straight up. Some machines will plunge downward approx. 1mm or more when it sees a G28 Z0. So it is safest first to give it a G91 so that the machine incrementally moves from it's last Z height position. Secondly, Giving a machine a G28 X0 Y0 allows safe celarance of the fixture or part for changing parts or loading the vise. You do not clarify your intentions at the end of the program so I am not sure why this is so important. Here's my best advise and the way I teach programming. If you want the machine to stay at the last point of operation. then just give it the following lines and delete sequence line N10.

N9 G91 G28 Z0
N11 M30

You say you want to delete the sequence line N9 also? Just how do you want to stop the program? Because if you are not careful, when you attempt to restart the program or depending on how you restart and what G codes are modal in the control or machine, you are almost guarenteed to crash eventually. This is why MasterCam does this. It is the best and safest way.

[luckyyyyyy]

Hi all,

Thanks alot for nice suggestion.

this method work... for adding the comment symbol before this line,,,

# pbld, n$, *sg28ref, "X0" "Y0." "A0", protretinc, e$

its works...because post doesn't compile this line....ok its fine...


but now in lathe post these two lines generate every time...



G28 U0. W0. M05
T0100




( i can understand first line ..its same like mill post Gcode ...tool move to zero point and spindle stop)
here now i also don't want this line..I tried to add in my lathe post but I think you can giude me better....the post is much different than MPFAN...so that's why i don't wana crash my machine...please tell me "rockchopper" ...which line I need to consider this time(lathe post)...if anybody know..please giud me...


and also you can see second line...that is " T0100 " ...tool number....why it creates everytime...how can I remove from post..??????????.kindly tell me ...??????????


thanks alot...

[luckyyyyyy]

----------------------------------------
#Retract to reference return
pbld, n$, `sgcode, psccomp, e$
if home_type = m_one, pbld, n$, *toolno, e$
#pcan1, pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.",
pnullstop, strcantext, e$
-----------------------------------------

this is lathe post code...I add comment symbol before the red line so its working...now its doesn't create this (G28 U0. W0. M05 ) line ....

what do you think "rockchopper" is it ok ....kindly tell me if it will create some problem in future...

---------------------------

if its ok ...then please tell me the second solution.... (T0100) tool number..

I dont want this tool number everytime at the end of Gcode like this...

G0 Z.1
G28 U0. W0. M05
T0100 ..................wana remove...
M30
%


thanks....