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:

Endless C-Axis Swiveling


Recommended Posts

1 hour ago, nickbe10 said:

Lock the C axis?

What kind of toolpath is it?

What kind of machine? 5 ax?

Where did you get your anti gravity device?

 

Cannot lock the C-Axis, it is a Swarf Toolpath but it acts dumb on the corners. Running on a Mazak 730-5X A/C Trunnion. Not sure what "device" but I am going with M.A.R.S!

Link to comment
Share on other sites

Sorry to say nature of the beast when a programmer makes the shape so close to singularity on the machine. This is where it is sometimes best to put a 5 or 10 deg tilt on the part in the setup to avoid this and get away from a singularity possible situations like what was created here.

  • Haha 1
Link to comment
Share on other sites
3 hours ago, 5th Axis CGI said:

Sorry to say nature of the beast when a programmer makes the shape so close to singularity on the machine. This is where it is sometimes best to put a 5 or 10 deg tilt on the part in the setup to avoid this and get away from a singularity possible situations like what was created here.

Oh so it's my fault huh? Thanks Ron!. Chuck Cook did mention that we should have a 5° tilt on the table, but what does he know....lol! You should see the Vericut singularity, fun stuff.

Link to comment
Share on other sites

Just an idea...When I have a machine where one axis goes ..let's say -5 to +180, to avoid the issue, I rewrite the axis limit from 0 to 180. After I finish I write back the limits. I use vectors for 5x programing , not direct machine axis.

  • Like 1
Link to comment
Share on other sites
3 hours ago, Grievous said:

Just an idea...When I have a machine where one axis goes ..let's say -5 to +180, to avoid the issue, I rewrite the axis limit from 0 to 180. After I finish I write back the limits. I use vectors for 5x programing , not direct machine axis.

Grevious,

Can you be a little more specific? Where do you set the limit, in the post or the operation?

Link to comment
Share on other sites
On 5/4/2019 at 10:35 AM, NOTW Programmer said:

Can you be a little more specific? Where do you set the limit, in the post or the operation?

As he is stated that he is using vectors for 5x paths, I would guess he is changing the machine axis limits in the machine parameters on the machine, not at the operation level in MCAM or post.  This will allow the machine to decide which way to go to get "proper" angles.

Kind of a clever solution if you ask me.  I have often wondered if using vector programming is actually better practice once you understand how to bend it to your needs.

Link to comment
Share on other sites
2 minutes ago, huskermcdoogle said:

I have often wondered if using vector programming is actually better practice once you understand how to bend it to your needs.

It can give you near total control of a 5X toolpath but can be a lot of work too.

MoldPlus makes a 5X add on for creating and modifying tool vector lines in Mastercam

It looks really sweet, but I have never had the opportunity to try it.

Link to comment
Share on other sites
1 hour ago, huskermcdoogle said:

As he is stated that he is using vectors for 5x paths, I would guess he is changing the machine axis limits in the machine parameters on the machine, not at the operation level in MCAM or post.  This will allow the machine to decide which way to go to get "proper" angles.

Kind of a clever solution if you ask me.  I have often wondered if using vector programming is actually better practice once you understand how to bend it to your needs.

Yes that is what I'm doing..I replaces in post the tool tip comp command with a call to a cycle in which I can set the limits I want...for example on a matsuura5X where A axis goes +11.5 to -111.5 I do this way:

TRANS_5A(0,-110.) ;TOOL TIP COMPENSATION ON
;************************************
REPEATB DATUM ;SET ACTIVE WPC
N3 G90 G0 X4.362 Y-6.9919 Z10. A3=0. B3=-.9918 C3=-.1277

...etc

The cycle looks this way..

PROC TRANS_5A(REAL UPPER_LIM, REAL LOWER_LIM)  SBLOF DISPLOF
;usage TRANS_5A(0,-90)
IF (UPPER_LIM > $TC_CARR32[1]) GOTOF ALLARM1
IF (LOWER_LIM < $TC_CARR30[1]) GOTOF ALLARM2

IF (UPPER_LIM==0)AND(LOWER_LIM==0)
ELSE
$MA_POS_LIMIT_PLUS[AX5]=UPPER_LIM  ;
$MA_POS_LIMIT_MINUS[AX5]=LOWER_LIM ;
ENDIF
$MC_TRAFO5_ROT_AX_OFFSET_1[0]=$P_UIFR[$P_UIFRNUM,A,TR]
$MC_TRAFO5_ROT_AX_OFFSET_1[1]=$P_UIFR[$P_UIFRNUM,C,TR]
NEWCONF  ;
STOPRE   ;
TRAORI
M132
M17

ALLARM1:
MSG("UPPER LIMIT IS > "<<$TC_CARR32[1]<<" /REPROGRAM THE COMMAND")
M00
M30

ALLARM1:
MSG("LOWER_LIM IS < "<<$TC_CARR30[1]<<" /REPROGRAM THE COMMAND")
M00
M30
  • Like 1
Link to comment
Share on other sites
On 5/3/2019 at 7:56 PM, NOTW Programmer said:

Oh so it's my fault huh? Thanks Ron!. Chuck Cook did mention that we should have a 5° tilt on the table, but what does he know....lol! You should see the Vericut singularity, fun stuff.

Not a matter of fault, but a matter of the process. The process being used puts the manufacturing process in a place where singularity is possible. The process has to either be setup in a way where that possibility is eliminated if not desired. The other option is to approach it differently from a programming stand point or use methods like be mentioned to eliminate that possibility also. I have done this very thing more than once and kicked myself every time I ran into it. We deal with it and do our best to not let is happen again, but yes when we program 5 Axis this happens from time to time.

  • Like 2
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...