topic Re: Has anyone actually got this software to work in Fusion Manufacture Forum

Has anyone actually got this software to work

Anonymous — Sat, 24 Oct 2020 19:22:52 GMT

As it seems no one has a Hurco post or has a Hurco lathe they have managed to get to work in ISNC

I opted to try the fanuc turning post, It produces code ,but not code that works , watching the videos of people who claim this stuff works, just simulating in fusion is not at a machine

it cannot seem to thread external i have tried a test part m28 x 1 spindle turning at rpm but thread cutting nowhere near 1mm per rev its almost

it will not tap in any cycle m29 gives an error not using a cycle it just pulls the tap out at the bottom of the spindle no dwell or reversal

I am havin serious doubt that this software is for little more than messing about on toy machines as it doesnt seem to do anything actually well.

Re: Has anyone actually got this software to work

Marco.Takx — Sat, 24 Oct 2020 21:09:58 GMT

Hi @Anonymous,

With Fusion 360 there is notting wrong.
Autodesk delivers basic post processors for free.
This doesn’t mean that they have to work directly.
It is possible that a basic post needs some modifications on it.

We delivered a few days ago a Hurco VCX600i post processor. Everything works great at that customer.

You can contact Cadac Group (send me a private message or email) to help you with a post processor or you can contact your Local Reseller in the link below how can help you.

HSM post adjustments needed? Find your right contact here.

If my post answers your question Please use Accept as Solution & Kudos This helps everyone find answers more quickly!

Re: Has anyone actually got this software to work

engineguy — Sun, 25 Oct 2020 01:16:46 GMT

@Anonymous

Think you need to be a bit more objective and less harsh, I am retired now but a couple of years ago I did CAM work for a company that had HURCO VMX64, VMX42 2 x VM10 mills and 3 x TM10 Lathes one with a magazine type barfeed and they all ran fine on ISO code from both Fusion and BobCAD softwares.

As @Marco.Takx rightly says most Post Processors don`t work 100% right out the box, mostly because they are not setup for all the different options that Machine Tool Builders offer with their products.

I have used numerous softwares over the years, MasterCAM, FeatureCAM, OneCNC, GibbsCAM etc, etc and I have never had a Post Processor yet that was 100% so have a little patience and ask some specific questions and you will get as much help as you need all for free, no maintenance fees or extra charges for Post Processor modifications here, be nice and you get nice back 🙂 🙂 🙂

Stay Safe

Regards

Rob

Re: Has anyone actually got this software to work

engineguy — Sun, 25 Oct 2020 02:23:50 GMT

@Anonymous

Just out of interest, have a look at the simple tapping cycle below and let us know what is wrong with it, check it against either your Winmax output or the conversational output at the control and I am sure that someone will have a go at producing a modified Fanuc PP that should work for you, the Fanuc is the nearest "out the box" PP for the Hurco Lathe, there are some really, really good Post Processor guys that often pop in to sort PP issues 🙂 🙂 🙂

It has the G95 for "Feed per Revolution" and I set a spindle speed of 400rpm to do an M8x1.25 thread and it has produced a Feed of 500mm/min which is correct, and a P250 which in Fanuc speak is 0.25sec dwell, anyway have a look, there may be lots wrong but if you don`t tell anyone then it is hard to fix anything 🙂

%
O6606
N10 G95 G18
N11 G21
N12 G50 S1000
N13 G28 U0. W0.

(TAP M8X1.25)
N14 T0202
N15 G54
N16 M8
N17 G98
N18 G97 S400 M3
N19 G0 X0. Z15.
N20 G0 Z5.
N21 Z15.
N22 Z5.
N23 G84 X0. Z-20. R5. P250 F500.
N24 G80
N25 Z15.

N26 M9
N27 G28 U0. W0.
N28 M30
%

Stay Safe

Regards

Rob

Re: Has anyone actually got this software to work

Anonymous — Sun, 25 Oct 2020 10:19:13 GMT

Hi Rob

I just tried that code and it comes up with an error for the p250 code we get similar code and can edit it manually to reproduce this everytime, Hurco say it should work but doesnt? so im actually baffled, as are they

My main issue at the moment is that when threading for example even if set to feed per rev for example if i set the machine to 100rpm for example and a 1mm pitch thread it doesn not travel at 1mm per rev and then decides to pull out at the end of the thread at maybe 0.005mmpr it literally takes 2 minutes to pul out 2mm or so it is in feed per rev mode

It would be nice also if feed was the pitch of the tap or thread also rather than the rpm of the spindle x 1.25??

It is not that i dont want to help myself but the help is very little use for writng or modifying the post and i certainly do nut understand the java

Re: Has anyone actually got this software to work

Anonymous — Sun, 25 Oct 2020 10:15:26 GMT

Marko how do we get in touch with you ?

Re: Has anyone actually got this software to work

engineguy — Sun, 25 Oct 2020 11:57:11 GMT

@Anonymous

The P250 should work, if Hurco agree it is correct then it may be a Parameter that needs changing in the HURCO control but they should know that, keep at them !!

As for the external threading it is outputting the correct feedrate for the Pitch, I did a simple external thread and set the pitch to 1.0mm and the output was F1., just changed the pitch to 2.0mm and the F changed to F2., that would suggest to me it is working OK, see code samples below for the external thread 🙂

%
O6607
N10 G95 G18
N11 G21
N12 G50 S1000
N13 G28 U0. W0.

(THREAD1)
N14 T0101
N15 G54
N16 M8
N17 G99
N18 G97 S280 M3
N19 G0 X40. Z5.
N20 G0 Z2.
N21 G92 X28.964 Z-10. F1.
N22 G0 X40. Z5.

N23 M9
N24 G28 U0. W0.
N25 M30
%

%
O6607
N10 G95 G18
N11 G21
N12 G50 S1000
N13 G28 U0. W0.

(THREAD1)
N14 T0101
N15 G54
N16 M8
N17 G99
N18 G97 S280 M3
N19 G0 X40. Z5.
N20 G0 Z2.
N21 G92 X28.964 Z-10. F2.
N22 G0 X40. Z5.

N23 M9
N24 G28 U0. W0.
N25 M30
%

That is the same program with only the pitch altered.

I`ll look into this some more when I get some time.

Stay Safe

Regards

Rob

Re: Has anyone actually got this software to work

engineguy — Sun, 25 Oct 2020 12:44:07 GMT

@Anonymous

Does your control work with a standard G4250 for the dwell ?? If so that can be easily done.

N23 G84 X0. Z-20. R5. G4250 F500.

Stay Safe

Regards

Rob

Re: Has anyone actually got this software to work

Anonymous — Sun, 25 Oct 2020 14:31:58 GMT

Hi Rob

no that presents a syntax error, Just bear with me i have spent 4 hours going through this just concentrating on rigid tapping and playing with various different lines of code to see what does and does not work

First I tried the code you sent, which didn't work for me , the spindle failed to rotate ccw and the P code is not recognised , but thank you it served as a valuable reference, the controller returns SCAN __ P CODE NOT USED

what did work

%
O6606
N10 G20 G40 G80 G90 G95 G18
N11 G21
N12 G92 S1000
N13 G28 U0. W0.
(TAP M8X1.25)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 G97 S400 M3
N19 G0 X0. Z15.
N20 G0 Z5.
N21 Z15.
N22 Z5.
N23 G95 G84.2 X0. Z-20. F1.25 S150
N24 G80
N25 Z15.
N26 M9
N27 G28 U0. W0.
N28 M30
%

what also did work

%
O6606
N10 G20 G40 G80 G90 G95 G18
N11 G21
N12 G92 S1000
N13 G28 U0. W0.
(TAP M8X1.25)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 G97 S400 M3
N19 G0 X0. Z15.
N20 G0 Z5.
N21 Z15.
N22 Z5.
N23 G95 G84 X0. Z-20. P1.0 F1.25 S150
N24 G80
N25 Z15.
N26 M9
N27 G28 U0. W0.
N28 M30
%

what did not work

%
O6606
N10 G20 G40 G80 G90 G95 G18
N11 G21
N12 G92 S1000
N13 G28 U0. W0.
(TAP M8X1.25)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 G97 S400 M3
N19 G0 X0. Z15.
N20 G0 Z5.
N21 Z15.
N22 Z5.
N23 G95 G84.2 X0. Z-20. P1.0 F1.25 S150
N24 G80
N25 Z15.
N26 M9
N27 G28 U0. W0.
N28 M30
%

program stops due to SCAN __ P CODE NOT USED error

%
O6606
N10 G20 G40 G80 G90 G95 G18
N11 G21
N12 G92 S1000
N13 G28 U0. W0.
(TAP M8X1.25)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 G97 S400 M3
N19 G0 X0. Z15.
N20 G0 Z5.
N21 Z15.
N22 Z5.

N23 M29
N23 G84 X0. Z-20. P1.0 F1.25 S150
N24 G80
N25 Z15.
N26 M9
N27 G28 U0. W0.
N28 M30
%

Program causes machine to stop dead and causes z axis following error .....servos stop

The below line is from HURCOs manual programming using fanuc mode B

Nnn M29
Nnn G84 X0.Z-.5 P1. Q.25 F.07692 S250 *** this does not work in fact it causes an axis following error and i have to restart the control if i use the M29 function *** I THINK THIS may be a major issue with the machine not fusion

It seems M29 is a horror story

the below is from the Rigid tapping page in Hurcos manual

G84.2 (or G84 M29) - Rigid CW Tapping
Rigid tapping allows the same hole to be tapped repeatedly with precision. The rigidtapping feature increases accuracy by synchronizing the rotation of the spindle with thefeed of the Z axis. G84.2 is used for right-handed tapping. M29 is required for Rigid
Tapping.
Default—No
Modal—Yes
Cancels:
•G80 - Canned Cycle Cancel (default)
•G81 - Drill Cycle
•G82 - Drill Cycle with Dwell
•G83 - Face Drilling with Pecks
•G84 - Face CW Tapping
•G85 - Boring Cycle
•G86 - Bore Rapid Out Cycle
•G87 - Side Drilling with Pecks/Dwell
•G88 - Side CW Tapping
•G89 - Side Boring Cycle
Format
G84.2 (or G84 M29) X ____ Z ____ P ____ Q ____ F ____ S ____
Parameters
•P—Seconds to dwell at bottom of hole
•Q—Distance for feed
•F—Feedrate
•S—Spindle speed
If P or Q are integers (no decimalpoint), the values will be dividedby 10000. For example, P10000 becomes P1.0.

Again it seems the P dwell function doesnt play well with G84.2

I will continue to experiment but will start a seperate thread for the threading cycle it might be useful for every one??...however

the below code is an example from a program i was sent , this works on the HURCO

N12 G76 P010060 Q250 R100
N13 G76 X26.774 Z-30.16 P613 Q250 F1.

using fusion (post FANUC TURNING.CPS) i cannot get it to populate PXX_XX_XX correctly

IT PRODUCES THE BELOW if i "USE CYCLE"

N22 G76 P001000 Q92 R0
N23 G76 X26.9 Z-33. P550 Q92 F1.5

if I don't use cycle it produces this

N21 X44.
N22 G1 X27.817 F5.
N23 G32 Z-33. F1.5
N24 X29.1 F1.5
N25 G0 X44.

Below is what a different post HURCO LATHE G33 threading iirc produces

N21 X80.711
N22 G1 X37.106 F1000.
N23 G33 Z-26.02 K2.
N24 G33 X39.414 Z-27.174 I2.
N25 G0 X80.711

the above is what one of the posts in fusion produces , which works also but its not the same post i used to get rigid tapping working to a degree ,

thanks

Tom

Re: Has anyone actually got this software to work

will_1 — Mon, 26 Oct 2020 16:02:19 GMT

Hi @Anonymous ,

I sent you a direct message with a link to a post for a Hurco lathe that I worked on a while back. It might be a better starting point than the Fanuc post you are currently working on. Would appreciate feedback.

Thanks,

Will