Any Luck from purchased post processor? 2

[uguser3]

We have purchased our first post from Siemens\UG for a 5 axis DMG. Over a year latter and it's usable only with some serious editing.At the same time we purchased a post for the same machine for Mastercam and it works flawlessly.Has anyone ever used a third party to write a post such as ICAM ?

 

[uguser3]

I'm impressed that your Mastercam guy got that one right

Yeah Bill us UG programmers laughed when they purchased it but now we check the UG output against the mastercam to try and get it right.We all are eating crow including the UG tech that was here two days working on the post.

Yes it is special output but not that uncommon anymore.
I can use the post builder for the generic stuff but writing the extra tcl commands is out of my leauge.
I'll PM you for your contact. Thank you

 

[Bugie]

Just out of interest what output do you need?

Is it something like this?

0 BEGIN PGM CAD MM
1 BLK FORM 0.1 Z X-30. Y-17. Z-37.657
2 BLK FORM 0.2 X+30. Y+17. Z+0.
3 FN 0: Q12 =+40000 ; RAPID FEEDRATE
; TOOL NUMBER 5 L0. R+5. : 16. FLAT ENDMILL
4 M300
5 TOOL CALL 5 Z S8000 ; 16. FLAT ENDMILL
6 CYCL DEF 32.0 TOLERANCE
7 CYCL DEF 32.1 T+5.
* - SWARF NEW TOOLPATH
8 LN X+11.256 Y-18.073 Z+150. NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX M3
9 CYCL DEF 303
Q394=1. ;Sampling
Q395=6000. ;max G value [0...10]
Q388=0. ;max G value for PgmSto
Q389=0.02 ;G message
; C+328.405 B-19.142
10 LN X+11.256 Y-18.073 Z+150. NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX ; C+328.405 B-19.142
11 M128
12 M126
13 LN X+11.256 Y-18.073 Z+150. NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX ; C+328.405 B-19.142
14 LN X+11.256 Y-18.073 Z+150. NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX ; C+328.405 B-19.142
15 LN X+11.256 Y-18.073 Z+4.926 NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX ; C+328.405 B-19.142
16 LN X+14.049 Y-19.791 Z-4.521 NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 FMAX ; C+328.405 B-19.142
17 LN X+16.842 Y-21.509 Z-13.968 NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 F1000 ; C+328.405 B-19.142
18 LN X+16.782 Y-21.022 Z-14.074 NX0. NY0. NZ0. TX-.2793100 TY+.1717975 TZ +.9447071 F1000 ; C+328.405 B-19.142

 

[uguser3]

Bugie,
No nothing like that, ours is ISO code



N1 T5
N2 G7 L1=1 A5=0.0 C5=0.0
N3 M57
N4 S12000 M3
N5 M8
N6 G0
N7 X3. Y1.5146
N8 Z.1
N9 G1 Z-.49 F10.
N10 X2.9854
N11 Y1.4854
N12 X3.0146
N13 Y1.5146
N14 X3.
N15 Y1.5771
N16 X2.9229
N17 Y1.4229
N18 X3.0771
N19 Y1.5771
N20 X3.
N21 Y1.6396
N22 X2.8604
N23 Y1.3604
N24 X3.1396
N25 Y1.6396
N26 X3.
N27 Y1.7021
N28 X2.7979
N29 Y1.2979
N30 X3.2021
N31 Y1.7021
N32 X3.
N33 G0 Z.1
N34 G174
N35 G7
N36 G141 L2=0 F2=15000.
N37 G0 B14.16 C174.981
N38 X2.6833 Y1.625
N39 Z.4
N40 X2.7354 Z.1046
N41 G1 X2.8415 Z-.4969 F10.
N42 X2.8414 Y1.5 Z-.4962
N43 X2.8413 Y1.4602 Z-.496 B14.58 C188.742
N44 X2.8412 Y1.4204 Z-.4953 B15.774 C200.8
N45 X2.841 Y1.3806 Z-.4942 B17.586 C210.508
N46 X2.8407 Y1.3407 Z-.4926 B19.852 C217.946
N47 X2.8939 Y1.3411 Z-.4946 B16.924 C230.451
N48 X2.947 Y1.3413 Z-.4958 B14.899 C246.434
N49 X3. Y1.3414 Z-.4962 B14.16 C264.981
N50 X3.053 Y1.3413 Z-.4958 B14.899 C283.001
N51 X3.1061 Y1.3411 Z-.4946 B16.924 C297.539
N52 X3.1593 Y1.3407 Z-.4926 B19.852 C307.946
N53 X3.1589 Y1.

 

[Jaydenn]

UGUSER3,

Is your posted example of code what you want?
Cause it looks like simple, boring, run-of-the-mill GCODE. Nothing special at all.

It's certainly NOT G141 type code.
G141 is 3D cuttercomp. It need contact point data, surface normal vector components and tool contact normal vector components(in certain situations).

Bugies code is what you want if you are using G141 for both iso or heidenhain conversational( i'm not talking about the setup stuff, i'm only refering to the xyz NxNyNz TxTyTz lines)

if your posted example is what you want... You only need a very basic post.

J

 

[uguser3]

Hi Jaydenn,
Very basic post... sorta. Ug has worked on last week several days, They tell me they are close so i'm hoping this nightmare will end.

G141= 3d cutcomp=yes.this is G141 on our control x,y,z tool contact points B&C are tool axis vectors or I J & K's can be used instead of B&C's

 

[jelmerra]

The 3d cutcom in millplus is a bit different from what other controllers require. The bugs in the contact data do make it quite a challenge to create a working postprocessor. Good luck, the siemens guys will get it right in time.

http://www.rouwe-analysis.info

 

[i0wa]

Best way to save your money is to get from anywhere documentation (if haven't yet) about NX and write the post by yourself, using help info. Tried by myself - it is real. Youy can set up 3D tool correction, but as for me, FANUC logics of correction is really poor. Its much faster to repost the program than do this correction. imho
With best regards
Yuri

 

[uguser3]

Yuri,
Thanks for the reply,I have been able to write all our Nx posts for all our other controls,but this one is a bit different.The G141 3d tool is alot more than just a 3d cutcomp.The cool thing about this machine is unlike the old controls where you had to know where your part is from center lines of your 4th and fith axis.You can set your mcs any where on your part post it ,then put and where on the table(4th axis )and run your program.thecontrol with the kinemetics of the machine does all the calculations instead of the post

 

[wmalan]

"The cool thing about this machine is unlike the old controls where you had to know where your part is from center lines of your 4th and fith axis.You can set your mcs any where on your part post it ,then put and where on the table(4th axis )and run your program.thecontrol with the kinemetics of the machine does all the calculations instead of the post"

At my last place we had a couple Hermles setup like that. The down side is they were the only 2 Heidenain machines in the shop and the only ones with that feature (probing program zero and tracking axis properly). When we had some mismatch on a couple impellers we were machining, none of us could figure out where the error was coming from.

Programming from a known position allowed us to deconstruct the error to find the problem. We ended up going back to the standard "Home is located here" to keep things simple.

--
Bill

 

[Bugie]

"The cool thing about this machine is unlike the old controls where you had to know where your part is from center lines of your 4th and fith axis.You can set your mcs any where on your part post it ,then put and where on the table(4th axis )and run your program.thecontrol with the kinemetics of the machine does all the calculations instead of the post"

Most new 5 axis mills work like this. It is called Tool centre point control

 

[wmalan]

"Most new 5 axis mills work like this. It is called Tool centre point control"

True. Just about all the new machines. That said, a LOT of the airframe shops (here is the US) are still using old iron and controls. The main issue is most all large airframe shops use a "failsafe" pin for their large multi-spindle gantries. Having the tool drive around the pin before cutting the part insures the proper tool is loaded. For that reason, the part must be oriented in a known position from that pin.

--
Bill

 

[Jules1968]

My company have recently become a VAR (value added re-seller) for Siemens in the UK, and we specialise in CAM rather than CAD. I am the post-processor writer and we can supply NX posts incorporating any of the functions that you mention. Contact me if you want any details. Julian.

 

[billytucker]

Good day I was just reading this post & found it interesting. I have just been transfered to a new facility within the company I work for & they have 2 Nocolas Correa 5-axis (A-axis rotary on X-axis, B & C axis nutating head ?) machines with the Heidenhain TNC-530 controls. I'm use to Fanuc type controls & Okuma, so the HeidenHain control is very new to me, learning curve time. I also have to learn NX6/NX5. The sample code Bugie posted looks very similar to the program files I was veiwing at work. Is this a readily available post for NX or is it one you built with the NX postbuilder ?. Also any links to training type materials for the Heidenhain control & NX would be appreciated. Sorry kind of long winded.

 

[jelmerra]

The heidenhain website has programming manuals and a programming station for download:

http://www.heidenhain.de/doku/tnc_guide/de/en/index/1242135142505/1242135142505.html

For an introduction to nx you could try CAST I think you need a license for that.

 

[uguser3]

Hello Billytucker,The guys at UG told me they had a post for Heidenhain conversational control ours is the iso version and they had not written one before.I received their last efforts back in November.We now have a uasable post with just a few minor tweaks needed.