Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Programming head-table 5-axis. Common practices.


?Mark
 Share

Recommended Posts

Okuma M800VH with Fanuc 31i-A5

 

Is there such a thing as "common practices"?

 

I'm new to this. I can make MC do what I want but the fanuc side/nc code gives us fits

 

Almost all our parts will have at least some 3+2. Increasingly, we have more and more simultaneous 5-axis tool-paths.

 

My questions:

1. Do you always use TCP "G43.4" on every part and tool-path?

2. If G54.4 WSEC is not included with the control (Fanuc 31i A5), how do you compensate for fixture errors? Re-posting?

3. If using G68.2 do you still need G54.2 ?

4. Do you ever really use regular G54, G55... offsets?

5. Look-ahead/smoothing. Which options do you use for contouring and which one for surfacing and simultaneous 5-axis milling? Do you really need them all?

G8 P1

G5.1 Q1 (AICC)

G5 P10000 (HPCC)

G5.1 Q3 M251-M255 (AI-NANO)

6. Use only inverse feed for all rotary and 5 axis moves?

7. Workpiece coordinate system. Parameter 19696 bit 5 (WKP) "0" or "1" ?

Setting it to "0" makes our G68.2 3+2 toolpaths work, but messes up 5-axis toolpaths

Setting it to "1" makes our 5-axis toolpaths work, but messes up regular G68.2 3+2 toolpaths

WTH

 

Does anyone have a sample MCX file (with 3 axis, 3+2 and 5 axis toolpath in one file) they can share with a correct nc code for this type of control? I feel that the support I'm getting with this new machine is below expectations...(

 

THANKS!!!

Link to comment
Share on other sites

Use G54.4 WSEC for fixture error. ( Only needed in case the part rotation is off. XYZ position isn't needed to be corrected with the 2 following codes )

G68.2 for all 2D, 3D, 3+2

G43.4 for all 5X simultaneous ( inverse time feed isn't needed as the TCPC command applys the programmed feedrate at the tool tip )

 

For highspeed command I would just go for the highest level.

 

Best regards

Mic

Link to comment
Share on other sites

Mic,

Great!

To clarify:

1. G68.2 and G43.4 will work with any positional adjustment but not rotational one. For rotational adjustment/error we need G54.4, right?

2. For any high speed control/look ahead you recommend to keep it simple and stick with G5.1 Q3 M251-M255 (AI-NANO)?

 

Thanks!

Link to comment
Share on other sites

Mic,

Great!

To clarify:

1. G68.2 and G43.4 will work with any positional adjustment but not rotational one. For rotational adjustment/error we need G54.4, right?

2. For any high speed control/look ahead you recommend to keep it simple and stick with G5.1 Q3 M251-M255 (AI-NANO)?

 

Thanks!

 

1. Yes G68.2 and G43.4 will compensate for ANY XYZ adjustment and you can also move your C-axis datum. Only need for G54.4 is if the AB rotation of the part is off.

2. Yes I guess AI-NANO is the highest Fanuc highspeed level so you can use this for all operations.

 

For 5X simultaneous you might also want to use the highspeed smooth TCP like Jeremy mentioned and the tool posture control

 

G43.4 L1 ( Smooth TCP ) P3 ( Tool posture control with smoothing)

 

L1 is smoothing of the vectors them self to remove jerks. Tool posture control ( P1 and P3 ) forces the tool to follow a ruled surface from one G1 point + vector to the next. P3 over P1 adds a smoothing to the complete path ( G1 path + vector path )

 

G43.5 is TCP based on IJK vectors while G43.4 is TCP based on machine angles. With G43.4 you can from the post define B+ or B- travel of the head ( in case your machine has both options ) With G43.5 the machine chooses B+ or B- depending what's closest to the current position, meaning you've less control.

 

In fact the manual from Jeremy is wrong. High-speed Smooth TCP (type 2) should read G43.5 and not G43.4 ( type 1)

 

Only benefit with type 2 is that you can use same program on different machine kinematic. E.g. AC table on one machine and BC table on another.

Link to comment
Share on other sites

Looks like G43.4L1 to turn smooth TCP on and G43.4L0 to turn it off.

 

Do you ALWAYS use TCP on 5-axis machines?

 

Thanks!

 

G43.4 L0 will only turn Smooth TCP off. TCP will still be on until you command a G49.

 

Only use TCP for 4X and 5X simultaneous work. For all other tasks G68.2 is the way to go. With G68.2 you can still use all normal 2D cycles ( hole cycles and cutter comp )

Link to comment
Share on other sites

G43.4 L0 will only turn Smooth TCP off. TCP will still be on until you command a G49.

 

Only use TCP for 4X and 5X simultaneous work. For all other tasks G68.2 is the way to go. With G68.2 you can still use all normal 2D cycles ( hole cycles and cutter comp )

This is our code:

 

 

(FINISH BACK CHAMFER)

N5 (1.500 DIA R.063 EM 3FL W/.610 LOC 6.450 REL MITSUBISHI AXD4000UR1503A)

T4

M6

T5

G0 G54 G90

G0 A-75. C0.

G68.2 X0. Y0. Z0. I180. J75. K0.

M68 (LOCK A)

M10 (LOCK C)

G43.4 H4 X-.9102 Y1.7957 Z10. S7643 M3

.

.

.

It's only a 3+2 cut but it still has both G68.2 AND G43.4 TCP

Is this wrong then?

 

Mic and Jeremy, You guys already helped me more then the support I got from the reseller...;)

Thanks!!!

Link to comment
Share on other sites

Of course it is. With no A or C movements G43.4 is basically just doing the tool length compensation and therefore you could just as well use G43. That way you're sure that you don't end up using some cycle which might conflict with TCPC as this function has some limitation in supported cycles/functions.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...