cantext

[Hacsta]

running v9.1sp2

 

i have 2 ops with the same tool, in 2nd op i use cantext to stop (M00) to add clamps etc.., then change nci tab i force tool change. then after i post it all out thier are M00 before every depth cut. I am using mpmaster post, is this a logged bug ? how quick is the fix? if any!!!!!!!!!

[Allan]

Not a bug, the force toolchange is doing a number on you. You could edit the ptlch0 postblock with a switch that would allow the M00 out only once, then reset the switch at the ptoolend postblock. Or you could use manual entry in between the operations where clamp moving is required and insert the M00 in the manual entry box.

 

HTH

 

Allan

[Hacsta]

so you say the force toolchange is doing the M00's at each depth cut? i read a post here about making a variable, counter and switching it on at ptlch0 and resetting it somewhere else . i couldn't get it to work..

 

is ptlch0 and ptoolend the only places i have to insert the switch.

 

i used the manuel entry before works good but looking for another way

[easystroke]

I found an easy way to do this. Create the first operation with the desired tool. Create the second operation. Instead of picking the new tool, pick a new tool that is identical. Right click on the tool to get the "define tool" window and change to the same tool number. You will have two tools with the same number that are identical. When you post it, mastercam will prompt you and ask if you want to create a tool change. Say yes and it will think it is doing a tool change and stop so you can reposition your clamps. Hope this helps.

[crazy^millman]

I have seen it before and I did edit the post ot not do this. It is fixable but I think easystroke had given you a good way if you want me to put up the code i will but it is not aq one liner if you understadn what I am saying.

 

Crazy Millman

[Hacsta]

Crazy Millman

if you would be so kind to put up the code that would be grrrrreat!

 

when i use canned text in the parameters page i use " stop before" and it put a M00 before the z retract home, then puts another M00 thats the one i want. where do i fix that at ?

thanks for the help

[Rekd™]

I use Misc Values to add M00's to my programs at the beginning of the op I want to stop at.

 

code:

---

%

O0001

(PROGRAM: T.NCF)

(MACHINE: PRESTAGE)

(MATERIAL: ALUMINUM INCH - 2024)

(TOOL 1: DIA 0.2500 1/4 CHAMFER MILL)

(TOOL 2: DIA 0.0200 #76 DRILL)

(OVERALL MAX Z.1)

(OVERALL MIN Z-0.25)

G00 G17 G40 G49 G80 G90 G20

T1

M01

( OPERATION: 1 DRILL )

M06(T1: 1/4 CHAMFER MILL)

(MAX-DEPTH | Z-0.1)

M03 S2139

G00 G90 G54 X0. Y0. A0.

G43 H2 Z.1 T2

G98 G81 X0. Y0. Z-0.1 R.1 F8.56

G80

G90

G91 G28 Z0.

G91 G28 Y0.

G90

M00 ( DO SOMETHING )

( OPERATION: 2 DRILL )

M06(T2: #76 DRILL)

(MAX-DEPTH | Z-.025)

M03 S5000

G00 G90 G54 X0. Y0. A0.

G43 H3 Z.1 T1

G98 G81 X0. Y0. Z-0.25 R.1 F4.28

G80

G91 G28 Y0. Z0.

G90

M06

M30

%

---

'Rekd

 

[ 10-16-2003, 09:16 PM: Message edited by: Rekd ]

[Hacsta]

reck'd,

i have'nt used misc values for stops, is their a way i could make misc value out put a position move to center table before the M00?

thanks for any help

[crazy^millman]

What about the mi10 that does the M00 before the operation why would that not work Hascta? all Mpmasters have this.

 

As far as going home you can also use the Ref position found on the paramter page to do this couldn't you.

 

I may be wrong and if I am Dave or Someone from emastercam will corretc me but they did the mi10 for the M00 because they were looking for the canttext to work a different way with their post.

 

Crazy Millman

 

[ 10-16-2003, 10:15 PM: Message edited by: Millman^Crazy ]

[Hacsta]

what i want to do is have the post out put a positon move to center table and a M00 before a op with the same tool as the previous op

 

T1 M06(TOOL)

GOO G90 G54 X 0 Y0 S5500 M03

G43 H01 Z1. M08

does the op

G00 Z1.

G28 Z0

CENTER TABLE

M00

T1 M06(TOOL)

GOO G90 G54 X 0 Y0 S5500 M03

G43 H01 Z1. M08

does other op

G00 Z1.

G28 Z0

M30

 

I'll try ref position in the morning thanks for the help

 

[ 10-16-2003, 10:35 PM: Message edited by: Hacsta ]

[crazy^millman]

Well you can make it defalut for all if you dont mind the extra moves all the time.

 

code:

---

 pretract        #End of tool path, toolchange              

sav_absinc = absinc

absinc = zero # for G53 move - not incremental

sav_coolant = coolant

coolant = zero

#cc_pos is reset in the toolchange here

cc_pos = zero

gcode = zero

pcan

pcan1, pbld, n, sccomp, psub_end_mny, e #(This line was also changed for the Fadals)

pbld, n, *sg91, sgcode, "G28", "Z0.", e #(This is what it should be for Fadals)

#pbld, n, sgabsinc, sgcode, "G53", "Z0", e #(This needed to be changed)

#pbld, n, "G28", "X0.", "Y0.", protretinc, e

#if abs(cabs) > 360 & nextop <> 1003, pbld, n, 'G28', protretinc, e

pcan2

absinc = sav_absinc

coolant = sav_coolant

---

Where I have the # at the pbld, n, g28 X0,Y0 just take out the # and it will do it every time now if you want ot be real slick you can put a if then for a mi6 and if you use the misc then it will put it in the program if you dont then it just like you have it. I know the theory but havign troublew getting the mi to work the way I want on soemthing else. I know one of the gru's will problay tell you in 2 sec but I have to play for hours and kinda doing about 10 things tonight so I will take another look this weekend if you dont get anything from someone esle cause if I can figure it I think I have got a trick post up my sleeve.

 

Crazy Millman

[Rekd™]

Yes, you can. I just have mine set to bring the Z to zero and the Y to the front for clamp changes, part flips etc.

 

You can have it do yours where ever you want.

 

Mine also prompts for a comment that it places with the M00, (leave blank for none). You could use this to type in a position during posting, or you could use Misc Values again to specify XYZA locations. Lots of ways to do that.

 

'Rekd

 

[ 10-16-2003, 11:22 PM: Message edited by: Rekd ]

[Rekd™]

LoL, Millman

 

'Rekd teh slow poke

[crazy^millman]

Hey Rekd 1900 that much closer to 2000 congrats bud. I am working on a post for the fadal that will allow you to do both subroutines as well as sub and I need a swtich for the sub_call that will require 2 sub-calls one that is the way it currently is then the other for the sub routines all the calls all the placement everything will need a switch control as well as if then equation at everyplace I need it to work properly. I also have already figured out how ot make all the fixed subroutines t owork wit hthis post and all canned cycles that work on a fadal. I can do the serilaztions routines as well as pocket rectangle/cicrle as well as bolt circle so now if I can get the subroutines working I can see some major advatagnes in keeping everything in one program format verse the mulit subprogram format and then other time I can where the other has it advantage.

 

Crazy Millman

 

Ps you calling me slow or what?

 

[ 10-16-2003, 11:38 PM: Message edited by: Millman^Crazy ]

[Hacsta]

WOW! Thanks for the code. I tried the misc values works good. the ref points is good too, everythings all good. i'm gonna try the "if then"

with the misc value too. this is great their is so much you can customize with mastercam just how you want it thank guys for the help i'll get back to you

[Rekd™]

Millman, looks like you're really enjoying working with posts. That's awsome. You know what's next... VB

 

Hacsta, you got that right, meng! I can't think of any other CAD/CAM package that has this kind of functionality.

 

'Rekd

[crazy^millman]

Ok I love working with the posts think that is very cool. Know learning anohter language like VB that is going to take some time. I can pretty much follw anything Rekd, Mick, Roger, Brian, Gismo, and the other Vb guys put up but without have a developer guide or programs real hard to just strike off from scratch and go buy what I need to do it. That kids a coming needs money and so does the current kid and this great State tax, Insurance helath and car, and fun fun.

 

Crazy Millman Peace out.

[Rekd™]

Millman, VB is easier to learn than Post. It's the same basic structure, but with VB you can use a much better IDE.

 

'Rekd

[Hacsta]

i did the "if then" with misc values to make the positioning move to the center of the table before the M00(which i use misc 10 for now thanks to mill man crazy) and also the force toolchange in the contour parameters page

 

i've never had a real post class, i just keep reading the mp post cdrom disc and keep asking questions here . you guys help out so much heres to you guys thanks for the help

 

[ 10-17-2003, 04:00 PM: Message edited by: Hacsta ]