Fixing problems with post to Anilam 1100M

[M3Shark]

Hi every one. I have recently been using an old Anilam 1100M with mastercam V9 at school. The person in charge of the machine shop never really uses the machine and does not know too much about operating it.

Anyway, I was supplied by him with a post processor that works well for the machine but has a few "glitches" that the more complicated my parts get, the more annoying the "glitches" become. I have looked into the Post i have, but can't really understand it, so i was hoping someone here might be able to help me fix the post.

The problems are:
1) for some reason it sets the Z drill depth to the feed height. Which results in me having to manually enter the depth of each hole on the machine, which is time consuming at just plain annoying.

2)When it goes to do a depth cut, it for some reason brings the end mill down diagonally from xyz 0, on all cuts after the first pass. This results more often than not on a chunk of my part being clipped on its way down. I can edit this out of code once it is on the machine, but it is really really annoying.

Anyway, If anyone wants to help me out, i can send them the post i am using. Any help or suggestions are appreciated.

Thank you.

[M3Shark]

does any one have any ideas?
Places to start?
any sites that have info about how post processors for Mastercam V9 work?


Thank you,

M3Shark

[Superman]

Copy your post into a compressed zip folder and attach to your next message

problem 1
We would need to see the post as to how it is set-up
this problem area is in the "drillcycle" section ( also state if it is happening on which or all cycles [spot, deep, peck, tap, etc)
---just recheck that you method of setting are correct, top of stock is not used in the calculation unless retract is in incremental ( can you attach a screen print if the setting parameter page to check how you've set the page )

problem 2
2 areas to look at , 1 being the "prapid" string or a parameter for "omit breakup of XYZ rapids" ( if it exists )

Probably would be best to put the zip file up

[M3Shark]

Thank you Superman.

Attached are the pst files that i got/have been using as well as screen shots showing the settings i have been using.

the cycle that i use is title Drill/Cbore. Results in a simple drill with no peck. I have not tried any other cycles.

Once again, thank you very much!!!!!

[Superman]

Looked at the post and your pictures

compare my mods to your current file
# means comment only
I have added 1 commented line regarding the XYZ breakup, un-comment it and check your results ( hopefully it will stop XYZ's in rapid )

Problem #1
I think it may be your settings in mastercam, it looks for an initial height for all your canned cycles which is the clearance plane but you have it turned off

Problem #2
have added a XY move after toolchange then Z on next line, in 2 places

also noticed you dont use the MISC INT (Miscellaneous Intergers ), your co-ordinate system is set by what is placed in MI#1, you seem to be locked to using only G53

[M3Shark]

Thank You So Much Superman!!

I will try to check it tomorrow, but might not be able to until Friday.

I think it may be your settings in Mastercam, it looks for an initial height for all your canned cycles which is the clearance plane but you have it turned off

What settings exactly might i have wrong in Mastercam? I am not sure what plane you are talking about. Are you talking about the top of stock plane? or the retract plane, or some other plane?

also noticed you dont use the MISC INT (Miscellaneous Intergers ), your co-ordinate system is set by what is placed in MI#1, you seem to be locked to using only G53

I have no idea what you are talking about here, I don't know what MISC INT's are, or what MI#1 is.

I am sorry if these are simple questions/things i should understand, but would you mind explaining them to me. There is no official class here at school for mastercam, so everything i know i have had to pick up from other people/myself/experimenting/ watching the very overly busy machine shop manager use Mastercam. So there are probably many things that i do not know that i should, but i am always eager to learn them.

[Superman]

Your pictures have returned

[M3Shark]

Wow, i can't believe i missed the giant button that says "clearance plane". So what exactly is the point of the clearance plane. I was taught to set the Retract plane slightly above the material, so what is the point to a clearance plane that retracts it even more? Where should i be setting the clearance plane to? Slightly above the retract plane?

Any chance you can explain to me what the options mean in the Misc Values are. Under work coordinates i guess i have two options, G92, and G54. What does this mean, what is the difference. Reference Return, G28 or G30, again what does that mean/difference? Incremental/Absolute Top layer? And a million different Misc. Integer and Misc Real options, all of them set to 0. What does this mean, and what are they used for?

Thank you again for all your help, i hope i am not asking to many questions for you...

[Superman]

For the drill cycles
Clearance plane--is the initial height the tool starts at and returns to at the end of machining the holes ( for newbie, this is should be above all features on the part and any clamping you have ). The "Use ... only at start and end.." forces the tool to stay at the "Retract" plane until the last hole

Retract plane--is the "start cycle from here" point ( usually output as Rvalue )

Top of stock--used if retract is in incremental or chamfering. It is a good idea to set it as the top of the hole

Depth--final depth of the cycle, plus the use of the calculator button beside it, plus the tip comp if enabled and set.

Dwell--how long you want the tool to "rub" at the bottom of the hole ( usually the time is in seconds )( I noticed in your post this is not enabled on all cycles )

Misc values
When checked ON, this lets mastercam know it is to use the values in this area
MI#1---this will set outputs to the NCfile that you want to use G92 or G54 work co-ordinate setting system ( this is covered by other threads )
MI#2-- you want absolute cordinates to be output
MI#3-- how do you want your machine to go to home position ( I guess you want G28 ( FANUC type codes ))

T/C plane
Enable this for setting up different setups or 4/5 axis work
eg "Top" only used for 3 axis work with the part set in the position you would be machining it
this area would need a lot of practice to fully understand it, play with the other stuff 1st before going for the harder bits.

Steve

[M3Shark]

Superman,
I got a chance to try out the new post today.

First the Good:
It does seem to have fixed problem number two!!!

However, it did not fix problem one, and created a new problem.

First, For some reason at the very beginning of the code, after tool 1, the code wants to send the machine to coordinate z 999.00. Which of course the machine tries to do and of course can't and results in a servo stop.

Second, The problem with hole depth has not gone away. If i try to use a clearance plane, then for some reason the machine now reads the clearance plane as the Z depth for the whole. While it reads the retract plane as the start hight, resulting in an error that reads ERROR: DEPTH MUST NOT BE HIGHER THAN START HEIGHT.

When i try the new post, but without the clearance plane, it sets the Z Depth to the retract plane like before.

MasterCam aslo gives an errors during Post error as follows.

Processing file with MPCRUN...
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg
Selector variable gcode = 1002.0
out of range for string select.
Postblock label ptlchg

Again, thank you for all your help!!!!

[Superman]

Sharkey
Can you post what is to be on the G81 line ?
Is there supposed to be 2 Zvalues or not ?
I get the 1st Z to be the depth value and the end one being the clearance Z value
or should the last Zvalue be before the G81 line ( red moved to blue position)

N0006 Z200.
N0007 G81 Z-5. R3. F75.0 Z200.

to get rid of the Z999
put a # on the front of the line ( 2 places )
ie

              #n, *z              #added 3/Sept/2009  # force out Z