5ax question

[ROB]

i did a search and found nothing about outputing

c/c on 5ax toolpath

i'm trying to cut an angle wall on a 5ax haas trunion

and need to use regrind 1/2 em's

so i need to use c/comp on the toolpath

so far i have not ben able to do it,

i can selected on the parameters but i wont output c/com when i post it

i try 5ax curve and 5ax swarf.

if any body have any input i will apreciated

i put a file on the ftp MCX2_Files/5axwall.mcx

if any body want to look at it thanks

 

x2mr2 sp1

windows xp 2gig ram

[SnowDay]

I would define the tool to its actual size in your tool library that should get the end result you are looking for with out using cutter comp. I don't know if cutter comp is possable on 5 axis toolpath.

[ROB]

i will think that if you have the c/comp option

in the parameters it should output c/comp

when posting

[Zoober]

It depends on your machine and post.

If your machine supports 3d CC, then it's possible. You are not generally going to get good results from 2D CC, because of the vectors going on in 5x work.

If your machine does support it, then you will prolly need some post mods.

[YoDoug®]

Haas does not support 3D cuttercomp. If the part geometry lets me I will use a tapered endmill for 5 axis swarf. that way small adjustments in TLO or tool length (depending on if the machine has dynamic tool length comp) will affect how much is cut off the wall. It is not a perfect solution but it does allow for a little adjustment at the machine with out having to repost.

[RObert TImby]

I have a vr-11 and i use Cutter comp but i have to turn it on under the misc. values buttton

 

here some reading i got from haas about 5x cutter comp:

 

G141 3D Cutter Compensation

This feature performs 3D cutter diameter compensation. The program is going to look like this:

 

G141 Xnnn Ynnn Znnn Dnnn Innn Jnnn Knnn

Subsequent lines can be of the form:

G01 Fnnn Xnnn Ynnn Znnn Innn Jnnn Knnn

or:

G00 Xnnn Ynnn Znnn Innn Jnnn Knnn

 

The 3D +/- G141 cutter compensation is not just for 5-axes work.

Some CAM systems are able to output the X, Y, and Z with values for I, J, K. The I, J, and K values tell the control the direction in which to apply the compensation at the machine.

The I, J, and K specify the normal direction relative to the center of the tool to the contact point of the tool in the CAM system.

The I, J, and K vectors are required by the control to be able to shift the tool path in the correct direction.

The value of the compensation can be in a positive or negative direction.

The offset amount entered in radius or diameter (Setting 40) for the tool will compensate the path by this amount even if the tool motions are 2 or 3 axes.

Only G00 and G01 can use G141.

D-code selects which offset to use.

G93 feed command is required on each block.

With a unit vector, the sum of I☻ J☻ K☻ must equal 1. (**☻-squared**)

Only the end-point of the commanded block is compensated in the direction of I, J, and K. For this reason this compensation is recommended only for surface tool paths having a tight tolerance (small motion between blocks of code).

For best results programming from tool center using a ball nose end mill.

 

For example:

T1 M06

G00 G90 G54 X0 Y0 Z0 A0 B0

G141 D01 X0.Y0. Z0. (RAPID POSIT WITH 5-AX C-COMP)

M11

M13

G01 G93 X.01 Y.01 Z.01 I.1 J.2 K.9747 F3250. (FEED INV TIME)

X.02 Y.03 Z.04 I.15 J.25 K.9566 F3400.

X.02 Y.055 Z.064 I.2 J.3 K.9327 F3227.

X2.345 Y.1234 Z-1.234 I.25 J.35 K.9028 F1580. (LAST MOTION)

G94 F50. (CANCEL G93)

M10

M12

G0 G90 G40 Z0 (RAPID TO ZERO, CANCEL 3 AXIS C COMP)

X0 Y0

M30

 

Note: G141 is a group 7 G code, G40 cancels G141, G91 is not compatible with G141, and G141 uses a D code same way that the G41 and G42 does.

 

hope it helps

[YoDoug®]

I thought the G141 was only for 3D not 5ax. I guess I have learned something new today.

 

I think the hard part would be to get the post to output the correct vectors since the part of the post that controls 5ax moves is protected. Also if the toolpath has wall and floor geometry selected how does MCX decide what vector to offset, from the wall or from the floor or a mix of both.

[RObert TImby]

Doug,

 

If you want it I have a pdf of information that is not included with the machine from Haas about 5ax haas trunions

 

rob

[Jrygus]

Hey Robert! Where did you get your post? I have a VR-8 and VR-9's and the Post i bought does not work well and does not support G141 comp. I am considering getting a new post for those machines.

[Zoober]

I think (not sure though) that NCI includes vector info for 5x work. The vectors are from plane coordinates and would determine tool control (vector IJK) for both floor and wall.

It would be the post that pulls that info from NCI to format into what the machine requires.

 

I think you are correct about the vector math being locked up Doug. I was told by our reseller that it is that way to keep us wannabe trigmasters from messing things up.

 

Mayhaps one of the IN-House 5x gurus can chime in and tell us if that is correct or not.