Parametric geometry

[AARONIS]

I've been using MasterCam for little over a year and a half now so I'm still a noob. Keep this in mind... Is there a way to make geometry parametric? I also program in Xialog Plus if you are familiar with SCM routers and I use parametric geometry in almost every program as to limit the number of programs I need. I would like to do something similar to this in MCAM. Is this possible or would it need to be done on the machine controller? FYI...this is going to be for a Heian router with a Fanuc controller.

[Lee.]

Are you talking like this,

 

Point "A" x23.125,y12.658,z4.289

 

Point "B" x102.35,y1.258,z5.468

 

?

[George_Gerhard]

Aaronis

You could purchase the user macro b option for your fanuc control and program parametrically.

 

rgds

George

[TK@PSG]

If your talking about this:

 

#100=3.245

G0 X#100

 

I don't think to many cam system can do it without an add on.

I create a simple file and do a mass edit turning all the X1.0's to X#100's

[AARONIS]

What I do in Xialog is reference the header line (dx,dy). I was just trying to find something as user friendly as this.

 

quote:

---

You could purchase the user macro b option for your fanuc control and program parametrically.

---

Thanks, I'll look into that. Are macros difficult to write though the fanuc controller?

[Chip-pan]

writtig a macro is like doing one of those tough word problems in high school algebra. Its all logic and following the logic

Look at CNC Concepts on the web. They have the best books Ive seen on programming macros.

 

Chip Pan

[AARONIS]

thanks

[Tim Johnson]

quote:

---

Are macros difficult to write though the fanuc controller?

---

YES,

It's much easier to write the macros on a pc and send them to the control. Seperate equations have to be put in all at one time also and some equations may be longer than the one line you have on the control.

[PE @ IHS]

The question was: Is there a way to make geometry parametric in Mastercam? The answer is no.

[AARONIS]

Actually my question was...

quote:

---

Is this possible (parametric geometry in MCAM) or would it need to be done on the machine controller?

---

So, being that I can't do this in MCAM do I have any other options? Other than the Macro B add on. My goal is to avoid writing 50-100 programs when I can write 2-3. I'm a fan of the K.I.S.S. method so when I can, I do. Thanks for everybody's help thus far....

[Tim Johnson]

What you can do is write the original file, set the operations in operation manager in incremental mode, import your new geometry, in operations manager click on the chain(s) and with the right mouse button click on the appropriate rechain choice, done.

 

It isn't parametric, but it would get the job done.

[Guest CNC Apps Guy 1]

quote:

---

...do I have any other options? Other than the Macro B add on. My goal is to avoid writing 50-100 programs when I can write 2-3...

---

If you want to program Parametrically, there is no avoiding Macro B. Essentially your programs will be looking like this;

 

code:

---

%

O2(DOING SOMETHING)

(CHANGE PARAM 6050=113)

G0G17G40G49G80G90

T1

M6

G0G90G54X0Y0S3000M3

G43H1Z.1

(X #24 = CENTER)

(Y #25 = CENTER)

(Z #26 = DEPTH)

(R #18 = RADIUS)

(Q #17 = SIDE CUT)

(S #19 = Z STEP)

(E #8 = PLUNGE FEED)

(F #9 = MILLING FEED)

(D #7 = FACTOR)

(K #6 = DIAMETER)

G113X0Y0Z.5R1.Q.3S.1E2.F20.D20K4.

G0G91G28Z0

G28Y0

M30

 

:9010

#102=0

#27=#5043

G0X#24Y#25

#102=0

#102=#102+#19+.1

N1G1Z-#102F#8

#32=#17/72

#33=0

#18=#18-#[13000+#7]

WHILE[#32LT#18]DO1

#30=[#32*COS[#33]]+#24

#31=[#32*SIN[#33]]+#25

G1#30Y#31F#9

#32=#32+[#17/72]

#33=#33+5

END1

#30=#18*COS[#33]

#31=#18*SIN[#33]

X#30Y#31

#29=#24-#30

#28=#25-#31

G3X#30Y#31I#29J#28

WHILE[#6NE#1]DO1

G3#30Y#31I#29J#28

#1=#1+1

END1

#18=#18*.9

#30=#24+#18*COS[#33+10]

#31=#25+#18*SIN[#33+10]

G3#30Y#31R#18

G0G91Z.1

G90X#24Y#25

IF[#102GE#26]GOTO3

#102=#102+#19+.1

IF[#102LT#26]GOTO2

IF[#102EQ#26]GOTO2

#102=#26

N2GOTO1

N3G0G90Z.1

M99

---

... and to do that Custom Macro B is REQUIRED.

[Tim Johnson]

While I was mowing my yard I was thinking while you can't make the geometry parametric, for a very similar part family you may be able to make a parametric program though the custom drill cycle basicly the same way as you would do a probe. It looks like you can have up to 20 parameters.

[Bruce Caulley]

Would it be possible to have to post output variables instead of co-ordinates???

 

You could then have a manual entry as your first operation that contained the "parametric" information you wanted and the post would do the rest.

 

Hhhhhhhmmmmmmmmmm

 

Bruce

[simon peter]

hi

 

i think that insted of makining lengthy program by using master cam why don't U use by applying G66.

 

Eg:

 

MAIN PGM.

 

T01M06

G54G90G40G80G00X0Y0

G43Z2.0H01

M03

M03S2500

G66P5000

X0Y0

X2.5Y0

X5.0Y0

G67

G90G00Z3.0M09

M05

M30

 

SUB;

O500

#1=0

N10

G01Z-#1F2

G01G91G41X1.0Y0D01F35

G03I-1.0J0F35

G40G00X0Y0

#1=#1+0.02

IF[#1LE1.0]GOTO10

G00G90Z1.0

M99

[Guest CNC Apps Guy 1]

Yes Tim You Are Correct, you could do this.

 

Nice idea, real nice. Not exactly what he was looking for but it would work and be parametric. No way to verify or backplot though but if you know exactly what you're looking for you can probably get by looking at the code.

 

You can also use a combination of the Custom Drill Cycles and Misc. Int/Reals.

 

JM2C

[Todd Tracey from Fastech]

Have you looked at the Mastercam ATP process? It was conceived for the Router market originally. Along with Excell to MC9 and other VBS scripts that already exist, you might find something to help. Run the mcamvb chook and look at the examples.

[AARONIS]

Ok, I think I've got enough info to take a stab at this. Thanks everyone for your input