Add Aggregate support to existing HAAS post

[Delcandoit]

Good Day,

 

I have searched the forums for this subject and I wasn't able to find what I was looking for, so here we go.

 

We run all HAAS in our shop and I currently have some solid 3, 4, & 5 axis posts that output what we need. We are getting 2 indexable aggregate heads and 1 Right Angle Head here shortly and I would like to add the correct functionality to our existing posts. I understand the programming of the heads and I have added an aggregate component to the Machine Definition within Mastercam. I have set my planes as I would with rotation Ex: WCS: Top C/T: Right. I have gotten an angled head within the toolpath and all of that good stuff. G19 posts in the safety line but reverts to G17 further down. It also doesn't seem to recognize the tool axis length. I converted a router post to Mill and it seems to output correctly but I'm not sure how to add that functionality to my existing posts. I know enough to be dangerous with posts and I pretty much just need a solid nudge in the right direction please.

 

N1 T14 M6

( T14 - 180.00 / 90.00 - STATION # )

( RAH TEST PATH )

(OP.1)

N2 G0 G19 G20 G40 G49 G80 G90

N3 G0 G90 G54 X1.9375 Y2.875 A0. S5000 M3

N4 G43 H14 Z2. T4

N5 M8

N6 Z.2

N7 G1 Z0. F5.

N8 G41 D14 Y3. F10.

N9 G17 G2 X2.5 Y3.5625 I.5625 J0.

N10 X3.0625 Y3. I0. J-.5625

N11 X2.5 Y2.4375 I-.5625 J0.

N12 X1.9375 Y3. I0. J.5625

N13 G1 G40 Y3.125

N14 Z.2 F15.

N15 G0 Z2.

N16 M9

N17 M5

N18 G91 G28 Z0.

N19 M1

[Colin Gilchrist]

Hi Del,

 

I started typing out a response to this, then realized it would be much better with pictures. Check out this PDF...

 

Thanks,

 

Colin

How to add Aggregate Head to Default Mill.pdf

[Delcandoit]

As usual Colin, you're awesome. I thought that I had done all of that already and no matter what Tool Axis Length I used there was no change in the code. I also got a G17 on line N9 in the sample code I posted. But, I have a feeling that I'm jumping the gun and that I need to read your well laid out tutorial a bit better and it will be clearer.

 

Thank you for responding and I hope that the everything is still going great for you in CT. Sorry for almost falling asleep in your Post class, jet lag and all lol.

[Delcandoit]

I've managed to get the logic implemented to our Mill post except for the "use_oal" logic. I'm having trouble tracking down where the math is done to offset the toolpath by the RAH gauge length and the tool overall length. I am using the MPRouter post as my inspiration and I have it narrowed down to the pxyzcout3 area, more specifically za and zshft. Does anyone have any reference documents they could point me towards for shift maps and mapping coordinates? We are an AS9100 shop with a very rigid QMS that dictates which code, and posts, we're allowed to use or I would just post with router and doctor the end code for HAAS. No doctoring allowed outside of Mastercam unfortunately. I have all of the values pulled for what I need, now it's just the vector math using our HAAS post. Any nudges and guidance is greatly appreciated.

 

Format:HTML Format Version:1.0 StartHTML: 165 EndHTML: 5913 StartFragment: 314 EndFragment: 5881 StartSelection: 314 EndSelection: 314

pxyzcout3 #Multisurf rotary axis motion & toolplane

if ra_type$ = 0 | fmtrnd(lng3(ra_svecx$) = zero),

[

#If you're not using the C-hook...

#your not getting C-Axis!

csav = zero

!cabs, !cinc

]

else,

[

if fmtrnd(vecz) = one,

[

c_tmp = atan2(m2$, m1$)

xshft = vequ(vzerox)

]

else,

[

csav = atan2(-ra_svecy$, -ra_svecx$)

ptfixx$ = vequ(vzerox)

axisx$ = vequ(caxisx)

tvecx = rotv(-csav, vecx)

csav = atan2(tvecy, tvecx)

axisx$ = vequ(caxisx)

c_tmp = csav

csav = atan2(vecy, vecx)

irotv = rotv(-csav, vecx)

bsav = atan2(irotv, krotv)

#Apply tool length

#(G43 is set with tool in Vertical for CA Head)

xshft = vequ(vzerox)

if ra_type$ = 1 | ra_type$ = 2, #If right angle or compound angle aggregate

[

if use_oal, zshft = tl_oal + gauge_length #Captured from 20007 & 20008 parameters

]

axisx$ = vequ(caxisx)

axisx$ = rotv(csav, baxisx)

ptfixx$ = vsub(xa, xshft)

xa = rotp(bsav, xa)

if set_g43_vert = 0, za = za + zshft

if set_g43_vert = 2 & ra_type$ = 1, za = za + zshft

]

csav = c_tmp

]

[Reko]

Yeah... I just use a router post and tweak it for the Haas, like you said.

 

I'll watch this thread for info on how to implement a RAH into a generic Haas post... hope you get it.

[Bill Craven]

On the FTP site ( Mastercam_forum/Training_file/) there is an aggregate tutorial (Aggregate Example.zip) that I did back in the X3 days and there is a converted router post in it that I used on a Haas. I don't remember how many other modifications I made to that post. Probably not very many.

 

I am sure that Colin's tutorial is more up to date, but there may be a pearl amongst the poo that you might find helpful.

 

There is also a sample toolpath and a listing of a couple of the "switches" in the post and how they affect the resulting NC file (use_ra_offs, and use_oal)

 

After having attended several of Colin's Post processor classes, I am sure that I could do a better job now. Kudos to Colin.

[DUC VU_45021]

hi everybody!

I have a cnc machine five axis(A,C) but I understand why it unknow G-code as G93 and G21, when in my programe have G93 and G21 so it alarm : IMPROPER G-CODE. how can i prepaire that alarm? . my machine is OHTORI KIKO OSU 545 FANUC 15M.

PLEASE HELP ME.

thanks for your help!

my email: [email protected]