will i ever get my code to look like this without editing?

[cherokeechief79]

heres a typical prog we run,all are structured the same.

 

O0176 (FIXED K CLAMP OP#1)

 

(MAT=3. WIDE X 5. LG X .500THK)

(XY 0=TOP LEFT CORNER)

(PCS TO FIT FIXTURE FOR NEXT OP)

 

 

(TOOL=1,.687 dia. Twist Drill )

(TOOL=2,.500 dia. End Mill RGH RAD=0)

(TOOL=3,.500 dia. End Mill FIN RAD=0)

(TOOL=4,.250 dia. SPOTDRILL RAD=0)

 

 

G00 G90 G80 G40 G17 G49

T1 M06

(--- 0.688 DIA. TWIST DRILL ---)

(DRILL BORE HOLES)

M01

S3000 M03

G54 M97 P1000

/ G55 M97 P1000

/ G56 M97 P1000

/ G57 M97 P1000

M09

 

G49 T2 M06

(---0.500 DIA. END MILL RGH ---)

(RGH 2.000 HOLE)

M01

S6000 M03

G54 M97 P2000

/ G55 M97 P2000

/ G56 M97 P2000

/ G57 M97 P2000

M09

 

G49 T3 M06

(---0.500 DIA. END MILL FIN---)

(FIN BORES)

M01

S6500 M03

G54 M97 P3000

/ G55 M97 P3000

/ G56 M97 P3000

/ G57 M97 P3000

M09

 

G49 T4 M06

(---0.250 DIA. SPOTDRILL ---)

(CHAMFERALL)

M01

S6500 M03

G54 M97 P4000

/ G55 M97 P4000

/ G56 M97 P4000

/ G57 M97 P4000

M09

 

G00 Z6.

G54 X7.5

G00 G91 G28 Z0 Y0 M05

G49

T1 M06

M30

 

N1000

(--- 0.688 DIA. TWIST DRILL ---)

(DRILL BORE HOLES)

G00 X1.4375 Y-0.95

M08

G43 H01 Z0.1

G98 G73 X1.4375 Y-0.95 Z-0.75 R0.05 Q0.1 F35.

X4.1245 Y-1.5

G80

G00 Z1.

M99

 

N2000

(---0.500 DIA. END MILL RGH ---)

(RGH 2.000 HOLE)

G90 G00 X1.4375 Y-0.957

M08

G43 H02 Z1.

Z0.05

G01 Z-0.6 F80.

G41 D02 Y-0.757 F45. (F55.)

G03 X1.4375 Y-0.757 I0. J-0.743

G01 Y-0.957

G00 Z1.

G40 X1.4375 Y-0.957

M99

 

N3000

(---0.500 DIA. END MILL FIN---)

(FIN BORES)

G90 G00 X1.4375 Y-0.847

M08

G43 H03 Z1.

Z0.05

G01 Z-0.7 F150.

G41 D03 Y-0.747 F40.

G03 X1.4375 Y-0.747 I0. J-0.753

G01 Y-0.847

G00 Z1.

G40 X1.4375 Y-0.847

X4.0745 Y-1.525

Z0.05

G01 Z-0.7 F150.

G41 D03 Y-1.575 F16.

G03 X4.1245 Y-1.625 I0.05 J0.

X4.1245 Y-1.625 I0. J0.125

X4.1745 Y-1.575 I0. J0.05

G01 Y-1.525

G00 Z1.

G40 X4.1745 Y-1.525

X-0.2042 Y0.3005

Z0.05

G01 Z-0.15 F150.

G41 D03 X0.2939 Y0.2569 F60.

G03 X0.3375 Y0.255 I0.0436 J0.4981

G01 X2.4557

X4.7759 Y-0.0711

G02 X5.3225 Y-0.6999 I-0.0884 J-0.6288

G01 Y-2.3001

G02 X4.7759 Y-2.9289 I-0.635 J0.

G01 X2.4557 Y-3.255

X0.4375

G02 X-0.1975 Y-2.62 I0. J0.635

G01 Y-0.38

G02 X0.4375 Y0.255 I0.635 J0.

G03 X0.4811 Y0.2569 I0. J0.5

G01 X0.9792 Y0.3005

G00 Z1.

G40 X0.9792 Y0.3005

M99

 

N4000

(---0.250 DIA. SPOTDRILL ---)

(CHAMFERALL)

G90 G00 X1.4875 Y-0.647

M08

G43 H04 Z1.

Z0.05

G01 Z-0.05 F65.

G41 D04 Y-0.597

G03 X1.4375 Y-0.547 I-0.05 J0.

X1.4375 Y-0.547 I0. J-0.953

X1.3875 Y-0.597 I0. J-0.05

G01 Y-0.647

G00 Z1.

G40 X1.3875 Y-0.647

X3.8745 Y-1.55

Z0.05

G01 Z-0.05

G41 D04 Y-1.575

G03 X4.1245 Y-1.825 I0.25 J0.

X4.1245 Y-1.825 I0. J0.325

X4.3745 Y-1.575 I0. J0.25

G01 Y-1.55

G00 Z1.

G40 X4.3745 Y-1.55

X0.2292 Y0.0541

Z0.05

G01 Z-0.055

G41 D04 X0.3288 Y0.0454

G03 X0.3375 Y0.045 I0.0087 J0.0996

G01 X2.441

X4.7466 Y-0.279

G02 X5.1125 Y-0.6999 I-0.0591 J-0.4209

G01 Y-2.3001

G02 X4.7466 Y-2.721 I-0.425 J0.

G01 X2.441 Y-3.045

X0.4375

G02 X0.0125 Y-2.62 I0. J0.425

G01 Y-0.38

G02 X0.4375 Y0.045 I0.425 J0.

G01 X0.5375

G03 X0.5462 Y0.0454 I0. J0.1

G01 X0.6458 Y0.0541

G00 Z1.

G40 X0.6458 Y0.0541

M99

[cadcam]

Now I have to say have you talked with your dealer to customize the post for your subs and layout?

 

The dealer is the palce to start if that does not work try contacting CNC.

[McRae]

The closest that you come up to this by yourself is by using MPSUBREP and then breaking everything into subprograms. Otherwise, you have to pay someone to make the changes for you.

[Scott Bond]

Hi

I had to make code look just ---EXACTLY-- like it came from a (1985) Gibbs post . I tried with the help of everyone in my roladex for about a year. Then we had a little talk that went like this,,

 

Do to the complains about my free service ,I will no longer provide any free service.

 

From that momoent forward the post has been fine.

 

[ 03-13-2003, 10:34 PM: Message edited by: Scott Bond ]

[Andy]

Oh, come on, cant you work for just one more year for free.

[connormac]

Hey Cherokee Chief,

 

I like how you set up your G55, G56 , & G57 with block delete(s). What can't you get your post to do and what are you posting to. While I was running my machine tonight I made my output look like yours. ( I think )

I don't know alot about MC but I can seem to figure out things in the post.

 

let me know

Kyle

[Guest]

Yes but it will require post editing.

 

It looks like several situations I have run into over the years usually in large corporations. The operator is inflexable.

 

So, you have choices;

You can learn how and spend the time.

You can sweet talk Scott, (sorry Scott).

You can try and talk your dealer into doing it. Do not be suprised if he will not, after all this has nothing to do with a functioning post and everything to do with personal prefrences.

You can hire someone and spend the money.

Before spending the money, you can explain to the operator how there will be no raises until the cost is recovered, of course it will then probably not be necessary.

 

Seriously, the posts can be made to do things like that. Sometimes the "why" is not as big as the cost. Also, most of what you want is already in many posts and may just need to be activated. The rest is not difficult. You may have to edit a few lines of text and make a few minor changes if the already existing code does not produce output that is suitable.

 

Good luck.

[DrewG]

When we were in class(Cherokee Chief & I), the teacher said he never saw a post like that used, and that it would be alot of work to get the post to look like that. We find this post very easy to navigate, simple to run a single test peice by hitting the block delete key on the control, and very easy to make an edit at the control for feeds and speeds. It seemed like in class the correct post would've been to copy each tool path for every offset used(ex.G54, G55, etc) instead of using sub's like in the above post. But you know how much a nightmare that is if your at the control trying to edit a feed or speed. If you were running 20 identiacl parts, you would be forced to edit the feed or speed 20 times, rather than just once in the sub. Another reason we use this type of post is to save memory. We do alot of engraving, and the post is super long. We wouldn't have enough memory in the control if we copied the tool path 20 times to do 20 parts.

Everyone that works with it loves it, so it's not a matter of "guys who just don't want to change", rather no one has shown us a post that's so easy to understand, and so easy to edit multiple parts right at the control. If we needed to add a few more parts on a fixture, we just add the more offsets. We sometimes will use a G10 at the top in order to load all the offsets everytime the job is started.

Why is this post with the subs so strange or foreign to everyone???

[MACHINEMASTERG]

hey drew and chief like andrew said try the mpsub rep its close to that code your looking for with some tweeks we have ours close to that but without the dlk delete we edited this to get the m97 insteed of m98its on this site and works great

[Guest CNC Apps Guy 1]

quote:

---

Why is this post with the subs so strange or foreign to everyone???

---

Subs are not strange or foreign to me, I just prefer not to use them because they are a Nightmare to manage at my work. We have a tough enough time keeping track of current part revisions out on the floor and their 2,3, or 4 assocoated programs for the different operations, let alone the BUNCH of subs that woudl go long with a situation like yours. Plus when we got our machines, (Mori Horizontals included) we had lots of extra memory installed. They have 1MB each. But as was said before, you have a few options,

 

quote:

---

You can learn how and spend the time.

You can sweet talk Scott, (sorry Scott).

You can try and talk your dealer into doing it. Do not be suprised if he will not, after all this has nothing to do with a functioning post and everything to do with personal prefrences.

You can hire someone and spend the money.

---

Why is that so hard to understand? I mean MPSubrep is a great starter but it won't get you there all the way, for that you need the services of a professional and it will cost. Maybe not a ton but it will cost.

[MACHINEMASTERG]

tweek the mpsubrep with m97 the local sub call all the sub programs will be under one program then call your dealer and have them fix up for you and your done finished no longer an issue this works great for us

[Rekd™]

I wrote Visual Basic program a few years back that does that; Take a normal single part program and seperate it into subs according to tools. Was kind of tricky to do, but the end result was fantastic, and I still use it today.

 

It takes this program...

quote:

---

%

O0001

(PROGRAM: JAWS5.NCF)

(MAR 14, 2003 06:53)

(MC8 FILE: 5 X 3.5 VISE JAWS)

(MACHINE: STANDARD)

(MATERIAL: ALUMINUM INCH - 6061)

(STOCK SIZE: X 5. Y 3.5 Z 1.)

(TOOL 1: DIA 0.4375 7/16 DRILL)

(TOOL 2: DIA 0.5000 1/2 FLAT ENDMILL)

(OVERALL MAX Z1.)

(OVERALL MIN Z-1.1514)

N1 G00 G17 G40 G49 G80 G90 G20

N2 M01

( OPERATION: 1 DRILL )

N3 T1 M06(T1: 7/16 DRILL)

(MAX-DEPTH | Z-1.1514)

N4 M03 S2514

N5 G00 G90 G54 X.5605 Y-.943

N6 G43 H1 Z1. M08

N7 G98 G83 X.5605 Y-.943 Z-1.1514 R.1 I.4 J.1 K.2 F18.1

N8 X4.4455

N9 G80

N10 M09

N11 G90

N12 M01

( OPERATION: 2 POCKET )

N13 T2 M06(T2: 1/2 FLAT ENDMILL)

(MAX-DEPTH | Z-1.01)

N14 M03 S6112

N15 G00 G90 G54 X.7005 Y-.943

N16 G43 H2 Z1. M08

N17 Z.1

N18 G01 Z-.8 F10.

N19 G03 I-.14 J0. F20.

N20 G01 X.5155 Y-.893

(OPERATION: 3 POCKET)

(T2: 1/2 FLAT ENDMILL)

N21 F10.

N22 G41 D2 X.4655 F20.

N23 G03 X.4155 Y-.943 I0. J-.05

N24 X.7055 I.145 J0.

N25 X.4155 I-.145 J0.

N26 X.4177 Y-.9679 I.145 J0.

N27 X.4755 Y-1.0086 I.0493 J.0086

N28 G01 G40 X.5247 Y-1.

N29 G00 Z1.

(OPERATION: 4 POCKET)

(T2: 1/2 FLAT ENDMILL)

N30 X4.5855 Y-.943

N31 Z.1

N32 G01 Z-.8 F10.

N33 G03 I-.14 J0. F20.

N34 G01 X4.4005 Y-.893

(OPERATION: 5 POCKET)

(T2: 1/2 FLAT ENDMILL)

N35 F10.

N36 G41 D2 X4.3505 F20.

N37 G03 X4.3005 Y-.943 I0. J-.05

N38 X4.5905 I.145 J0.

N39 X4.3005 I-.145 J0.

N40 X4.3027 Y-.9679 I.145 J0.

N41 X4.3605 Y-1.0086 I.0493 J.0086

N42 G01 G40 X4.4097 Y-1.

N43 G00 Z1.

(OPERATION: 6 POCKET)

(T2: 1/2 FLAT ENDMILL)

N44 X.5755 Y-.943

N45 Z.1

N46 G01 Z-1.01 F10.

N47 G03 I-.015 J0. F20.

N48 G00 Z1.

(OPERATION: 7 POCKET)

(T2: 1/2 FLAT ENDMILL)

N49 X4.4605

N50 Z.1

N51 G01 Z-1.01 F10.

N52 G03 I-.015 J0. F20.

N53 G00 Z1.

(OPERATION: 8 POCKET)

(T2: 1/2 FLAT ENDMILL)

N54 X.5545 Y-.938

N55 Z.1

N56 G01 Z-1.01 F10.

N57 G41 D2 X.5495 F20.

N58 G03 X.5445 Y-.943 I0. J-.005

N59 X.5765 I.016 J0.

N60 X.5445 I-.016 J0.

N61 X.5453 Y-.9479 I.016 J0.

N62 X.5516 Y-.9511 I.0048 J.0015

N63 G01 G40 X.5563 Y-.9496

N64 G00 Z1.

(OPERATION: 9 POCKET)

(T2: 1/2 FLAT ENDMILL)

N65 X4.4395 Y-.938

N66 Z.1

N67 G01 Z-1.01 F10.

N68 G41 D2 X4.4345 F20.

N69 G03 X4.4295 Y-.943 I0. J-.005

N70 X4.4615 I.016 J0.

N71 X4.4295 I-.016 J0.

N72 X4.4303 Y-.9479 I.016 J0.

N73 X4.4366 Y-.9511 I.0048 J.0015

N74 G01 G40 X4.4413 Y-.9496

N75 G00 Z1.

N76 M09

N77 G91 G28 Y0. Z0.

N78 G90

N79 T1 M06

N80 M30

%

---

...and converts it to this, with NO MANUAL EDITS!

 

 

quote:

---

%

O0001

(PROGRAM: JAWS5.NCF)

(MAR 14, 2003 06:53)

(MC8 FILE: 5 X 3.5 VISE JAWS)

(MACHINE: STANDARD)

(MATERIAL: ALUMINUM INCH - 6061)

(STOCK SIZE: X 5. Y 3.5 Z 1.)

(TOOL 1: DIA 0.4375 7/16 DRILL)

(TOOL 2: DIA 0.5000 1/2 FLAT ENDMILL)

(OVERALL MAX Z1.)

(OVERALL MIN Z-1.1514)

N1 G00 G17 G40 G49 G80 G90 G20

N2 M01

( OPERATION: 1 DRILL )

N3 T1 M06(T1: 7/16 DRILL)

(MAX-DEPTH | Z-1.1514)

N4 M03 S2514

N5 G00 G90 G54 X.5605 Y-.943

N6 G43 H1 Z1. M08

G54 G17 X.5605 Y-.943

M98 P3

/ G55 G17 X.5605 Y-.943

/ M98 P3

/ G56 G17 X.5605 Y-.943

/ M98 P3

/ G57 G17 X.5605 Y-.943

/ M98 P3

N10 M09

N11 G90

N12 M01

( OPERATION: 2 POCKET )

N13 T2 M06(T2: 1/2 FLAT ENDMILL)

(MAX-DEPTH | Z-1.01)

N14 M03 S6112

N15 G00 G90 G54 X.7005 Y-.943

N16 G43 H2 Z1. M08

G54 G17 X.7005 Y-.943

M98 P4

/ G55 G17 X.7005 Y-.943

/ M98 P4

/ G56 G17 X.7005 Y-.943

/ M98 P4

/ G57 G17 X.7005 Y-.943

/ M98 P4

N76 M09

N77 G91 G28 Y0. Z0.

N78 G90

N79 T1 M06

N80 M30

 

O3 ( SUB NUMBER: 3 )

N7 G98 G83 X.5605 Y-.943 Z-1.1514 R.1 I.4 J.1 K.2 F18.1

N8 X4.4455

N9 G80

M99

 

O4 ( SUB NUMBER: 4 )

N17 Z.1

N18 G01 Z-.8 F10.

N19 G03 I-.14 J0. F20.

N20 G01 X.5155 Y-.893

(OPERATION: 3 POCKET)

(T2: 1/2 FLAT ENDMILL)

N21 F10.

N22 G41 D2 X.4655 F20.

N23 G03 X.4155 Y-.943 I0. J-.05

N24 X.7055 I.145 J0.

N25 X.4155 I-.145 J0.

N26 X.4177 Y-.9679 I.145 J0.

N27 X.4755 Y-1.0086 I.0493 J.0086

N28 G01 G40 X.5247 Y-1.

N29 G00 Z1.

(OPERATION: 4 POCKET)

(T2: 1/2 FLAT ENDMILL)

N30 X4.5855 Y-.943

N31 Z.1

N32 G01 Z-.8 F10.

N33 G03 I-.14 J0. F20.

N34 G01 X4.4005 Y-.893

(OPERATION: 5 POCKET)

(T2: 1/2 FLAT ENDMILL)

N35 F10.

N36 G41 D2 X4.3505 F20.

N37 G03 X4.3005 Y-.943 I0. J-.05

N38 X4.5905 I.145 J0.

N39 X4.3005 I-.145 J0.

N40 X4.3027 Y-.9679 I.145 J0.

N41 X4.3605 Y-1.0086 I.0493 J.0086

N42 G01 G40 X4.4097 Y-1.

N43 G00 Z1.

(OPERATION: 6 POCKET)

(T2: 1/2 FLAT ENDMILL)

N44 X.5755 Y-.943

N45 Z.1

N46 G01 Z-1.01 F10.

N47 G03 I-.015 J0. F20.

N48 G00 Z1.

(OPERATION: 7 POCKET)

(T2: 1/2 FLAT ENDMILL)

N49 X4.4605

N50 Z.1

N51 G01 Z-1.01 F10.

N52 G03 I-.015 J0. F20.

N53 G00 Z1.

(OPERATION: 8 POCKET)

(T2: 1/2 FLAT ENDMILL)

N54 X.5545 Y-.938

N55 Z.1

N56 G01 Z-1.01 F10.

N57 G41 D2 X.5495 F20.

N58 G03 X.5445 Y-.943 I0. J-.005

N59 X.5765 I.016 J0.

N60 X.5445 I-.016 J0.

N61 X.5453 Y-.9479 I.016 J0.

N62 X.5516 Y-.9511 I.0048 J.0015

N63 G01 G40 X.5563 Y-.9496

N64 G00 Z1.

(OPERATION: 9 POCKET)

(T2: 1/2 FLAT ENDMILL)

N65 X4.4395 Y-.938

N66 Z.1

N67 G01 Z-1.01 F10.

N68 G41 D2 X4.4345 F20.

N69 G03 X4.4295 Y-.943 I0. J-.005

N70 X4.4615 I.016 J0.

N71 X4.4295 I-.016 J0.

N72 X4.4303 Y-.9479 I.016 J0.

N73 X4.4366 Y-.9511 I.0048 J.0015

N74 G01 G40 X4.4413 Y-.9496

N75 G00 Z1.

M99

%

( File Size: 2.6kb )

( File Length: 131 lines )

( File Modified 3/14/2003 at 6:54:39 AM )

---

 

[ 03-14-2003, 09:59 AM: Message edited by: Rekd ]

[MACHINEMASTERG]

nice job rekd ....there you go chief now pony up the bucks $$$$$$

[connormac]

I made my program look like that by adding a few block delete(s) to my post.

[cherokeechief79]

$?????????????????

 

ISNT THAT SOMETHING MY VAR SHOULD BE ABLE TO HANDLE FOR ME?

does support for the product also fall short of smartcam?

[Guest CNC Apps Guy 1]

quote:

---

ISNT THAT SOMETHING MY VAR SHOULD BE ABLE TO HANDLE FOR ME?does support for the product also fall short of smartcam?

---

You should have had Posts as part of your purchase. Lack of planning on your part should not constitute an emergency (that THEY are going to have to foot the bill for) on your reseller's part. Now you're being unreasonable. At first I just though you were picky( no biggie, it's your money - or your company's money), now I know your'e not only picky but you're ureasonable.

 

SmartCAM support???? Are you on DRUGS????? Where's the support NOW????? Where's the development NOW???? Where's the SmartCAM development going in the FUTURE??????

 

That's what I thought!

 

OUT!

[Guest CNC Apps Guy 1]

And another thing, the quality of your posts here is severly lacking. You have nothing good to say, it's just bash, bash, bash. My SmartCAM this, My SmartCAM that. You know what, just go back to it. Stay in the past because obviously you can't handle the future. We've tried to help you out but you're hopeless. You'll get no further help from me.

 

Some customers just are not worth having, and you're one of them. Why don't you at least tell us what state you're from? Afraid of the backlash?

 

OUT!

 

[ 03-14-2003, 03:05 PM: Message edited by: James Meyette ]

[Trevor Bailey]

Now the fun begins . Can't wait to see the reply to this one for James. I doubt the guy is around for much longer.

 

On a serious note, give your dealer a chance to help you with your problem(NOT) before you start bashing anyone/anything. From what I have seen in this forum, I do not blieve that there has been one question that was asked go unanswered oR taken care of when IT WAS ASKED NICELY.

 

Good luck to you anyhow.

[Rekd™]

quote:

---

$?????????????????

 

ISNT THAT SOMETHING MY VAR SHOULD BE ABLE TO HANDLE FOR ME?

does support for the product also fall short of smartcam?

---

LOL!!!

 

What a maroon.

 

I'll address these issues one at a time, so as not to confuse or mislead anyone...

 

Money? Um... YEAH!! (duh!) You think everything is free? Notice: Free Services have been canceled due to complaints about Free Services. (Good Job, Stupid! Hope you're happy now.)

 

VAR Supporting Posts? Um... Yeah, within reason. If it is functional, the VAR's commitment stops there. (See "Money" above, stupid.)

 

Support? Um... The only support you'll get from me from now on is my hand supporting the back of your head while I smash your computer into your face. If you can find ANY cad/cam software that has the support network and following of users willing to help (most) users that MC has, I'll kiss your stinky feet.

 

HTH, stupid!

 

'Rekd

 

[ 03-14-2003, 03:30 PM: Message edited by: Rekd ]

[McRae]

I know what the user is reffering to. The posts in Smartcam are far simpler than Mastercam and even a novice user could make significant changes with minimal assistance. The dealer network in its time was superior to Mastercam and the quality and level of professionalism was second to none. James - we have someone here who is trying to make a concerted effort at changing, live with the criticism for now and once the user is familiar with the software and is still impudent with respect to us - then roast away. I notice that Kathy was saved the blood bath on her negative comments!

 

I went thru the same pain as this user so please - patience and understanding is warrented, after all in his mind (and in mine on the odd occasion) he has had to take a step back in using MC.

[Guest CNC Apps Guy 1]

quote:

---

I notice that Kathy was saved the blood bath on her negative comments!

---

But she is a contributing member. She doesn't come in here specifically with the intent of bitching and moaning like this pansy @$$.

 

quote:

---

patience and understanding is warrented,

---

I think we've been quite patient with his wining @$$ and I've had it and I don't think I'm alone either.

 

quote:

---

James - we have someone here who is trying to make a concerted effort at changing,...

---

BULL $#!+ !!!!!!!!!!

[cherokeechief79]

im from nj ,im not leaving,and childish comments like james likes throwin at me dont bother me either.

ive never paid for getting a post to work to my liking(but maybe now thats the norm)

the post that rekd posted was very good and similar to my style(i still dont know why the output i want is so out of the ordinary)but it seems it would have to be posted and then run again somehow to convert it.much like we do now on our seimens 840 c controller with a fanuc converter.

i WAS told that mc had a post that was very similar to what i wanted,but when i went to training was told that this style was very unusual and would require a lot to get it the way i want it.

ive contributed a lot of useful info on my other forums and in time will do here also.

if i didnt feel i had to move on to newer and better things i would have just stuck with sc.

one way or another i will learn this new system (with or without YOUR help)

these 2 systems are very different and im not bashing either but if i cant even say how something was easier (like tweakin a post)without someone getting offended then i guess ill just have to call my var for info without using this forum.

either way im not leaving.

im just not used to the way you guys handle things here.

[cherokeechief79]

quote:

---

quote:

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

I notice that Kathy was saved the blood bath on her negative comments!

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

 

But she is a contributing member. She doesn't come in here specifically with the intent of bitching and moaning like this pansy @$$.

---

tell me just how you think i can be a contributing member with only 4 posts so far?do you really think i could give you usefull info on mc yet?

 

as far as 'pansy @$$' goes.(thats just childish crap that i really didnt expect here)

i guess ill just have to learn who is helpfull and who isnt here.

[Allan Brown]

Always on a Friday at 5:00pm EST it seems...

 

Q: Will I ever get my code to look like this without editing?

 

A: Wrong question, because your own solution decisions and steps factor in.

 

Like "Will I ever walk through the door?" Don't know, but certainly the door can be walked through.

 

Your desired code format is achievable. Probably in 5 to 10 minutes in the hands of an experienced post writer with an understanding of your application - less time than it took to read this thread. Getting there may involve a few steps, like paying your reseller or subcontractor of theirs if this level of post customization was not part of your deal.

 

The structural changes you need go beyond offering up variable names and post code snippets here. It sounds like you need to contact your reseller. They always have the option of contracting the work out if necessary. Just letting you know what's possible. Thanks for toughing it out here.

[CAM-mando]

Im a new member here also though Ive been using MC for 7 years and Smart Cam for 5 before that. I understand the frustration of Cherokee Chief because I got the same deal when I purchased MC. "Yeah yeah yehah we got posts for everything what we dont have we can get yada yada yada." But the hankshake deal the VAR gives you isnt real firm. Se la vie . I like a challange and get mad and figure the stupid post language out enough to get the post how I want it.

 

Coming from a program like Smart Cam it is a bit of a shock seeing the complexity of the MC post. So the guy asks a few questions Beenie boy over there gets his panties in a bunch . The guy's expressing a little frustration with the transition. He bought his software, paid for training, and your gonna call him cheap because hes trying to figure out how to get his code the way he wants it ??

 

And furthermore Ive met quite a few instructors who know MasterCam but dont know CNC. For an instructor to describe the cited code as odd just shows his inexperience with CNC code.

 

Now Im not bashing here honest ... but ... by now post creation ought to be an interactive Q & A drag and drop process. (Actually it is if you want to buy a $10,000 3rd party app like intercim.) But its not within the scope of CAM packages (yet).

 

Anyway thats all from me.