topic Re: Fanuc 3T Post Processor Needed in HSM Post Processor Forum

Fanuc 3T Post Processor Needed

Anonymous — Sat, 12 Mar 2016 06:39:42 GMT

Like the title says. I have a Miyano BNC34T (1985)

It utilizes a simple Fanuc 3T Control.

Has a RS232 serial port. I have made the switch from a popular CAD/CAM software wich ryhmes with the latter part 🙂

Will the Generic Fanuc Lathe Post Processor output the correct G-Code?

I have already noticed, it continually sets my G50 at 6,000 even if I have the CSS set at 3,000 or If I disable use CSS it still sets the G50 to 6000 even if my spindle speed is 3,000. Guess if I have CSS disabled it's a mute point.

Anyhow, this is my first post and most definitly not my last.

Any help would be appreciated.

Re: Fanuc 3T Post Processor Needed

HughesTooling — Sat, 12 Mar 2016 10:40:08 GMT

@Anonymous wrote:

I have already noticed, it continually sets my G50 at 6,000 even if I have the CSS set at 3,000 or If I disable use CSS it still sets the G50 to 6000 even if my spindle speed is 3,000. Guess if I have CSS disabled it's a mute point.

Anyhow, this is my first post and most definitly not my last.

Any help would be appreciated.

On the post dialog under Properties look for the option maximumSpindleSpeed and set it to 3000.

Another option to might need to experiment with is type (options are A,B,C), for my 210iT I need to set it to B to get the correct format for threads, setting the spindle max speed, etc.

Mark

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 07:14:01 GMT

I was reluctant to make the jump to Fusion. So far I have spent 2 days and nothing but headaches.

When using the Generic Turning Fanuc Post - It doesn't output Canned Cycles such as G71?

Its generating code for each pass?

How is Fusion Running on Macbooks? I have some weird stuff going on.

Re: Fanuc 3T Post Processor Needed

Laurens-3DTechDraw — Sun, 13 Mar 2016 07:42:00 GMT

No, it will not output canned cycles for turning. So yes you see every pass.

What headaches do you have?

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 07:51:41 GMT

I am sure most of the headaches are all on my end.

How reliable has Fusion been running on Macs?

It's my only laptop so I would prefer to use the Mac - So I can easily get my programs onto my different machines.

I have an older Fanuc 3T Controller. I am new to turning and CNC in general. Is there anything I should modify on the Generic Turning Fanuc PP? I see so many different options Such as Type A etc... Not sure what 3T is? Guess I will just need to start sending programs to the controller and doing some dry runs to see what I am getting.

Also how do I add a custom PP file that someone has created and shared with me?

Once I PP it opens up a program called brackets....is that where I communicate VIA RS232 to my Lathe?

Sorry this is all new to me as I was using another CAD/CAM package prior and am trying to give this a shot.

Re: Fanuc 3T Post Processor Needed

Laurens-3DTechDraw — Sun, 13 Mar 2016 08:53:18 GMT

There is a thread here on where to store custom posts: http://forums.autodesk.com/t5/post-processors/where-to-put-cps-files-for-fusion-360/td-p/6093729

Sadly there is no DNC(RS-232) software with the program. There is with Inventor HSM and HSMWorks, but since that(called HSMEdit) doesn't run on MAC they decided to not ship it with the software.

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 09:09:58 GMT

Ok,

1.) So I assume once I generate my G-Code I would need to save that and open into a 3rd party .NC editor so I could transfer Via RS-232

2.) I have Fusion Installed on my Home Computer as well. One thing, every single time I click X or Close Fusion 360 I get (Not Responding) This happens everytime I try to shut it down. Have to enter Task Manager and force quit?

Thanks for the speedy replies. Hoping to get the bugs ironed out and look forward to learning something new!

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 18:59:54 GMT

Additional Quirks

1. Under Cam I have Selcted "dont go home"

2. I also have selected "feed per revolution"

Yet when I PP the Tool Paths, I keep getting a G28 U0 at the end of each operation

I also get a G98 at the top of the Processor?

This is Using the General Turning Fanuc PP Model A (I did try changing to B, and that cleared the G98, But not the G28 U0)

%
O1001
N10 G98 G18
N11 G20
N12 G50 S3000
N13 G28 U0.

(FACE1)
N14 T0101
N15 G54
N16 M8
N17 G99
N18 G97 S1000 M3
N19 G0 X1.3 Z0.0466
N20 G1 X0.6131 F0.005
N21 X0.5 Z-0.01
N22 X-0.0625
N23 X0.0506 Z0.0466
N24 G0 X1.3
N25 G28 U0.

(DRILL1)
N26 M1
N27 T0303
N28 G54
N29 G98
N30 G97 S750 M3
N31 G0 X0. Z0.03
N32 G17
N33 G0 Z0.02
N34 Z0.03
N35 Z0.02
N36 G83 X0. Z-0.7501 R0. Q0.16 F2.25
N37 G80
N38 Z0.03
N39 G28 U0.

(PROFILE2)
N40 M1
N41 T0202
N42 G54
N43 G99
N44 G97 S500 M3
N45 G0 X0.58 Z0.1969
N46 G0 Z0.0662
N47 G1 X0.5731 F0.005
N48 X0.46 Z0.0096
N49 Z-0.7929
N50 X0.5392
N51 X0.6523 Z-0.7363
N52 G0 Z0.0662
N53 X0.5111
N54 G1 X0.398 Z0.0096 F0.005
N55 Z-0.7929
N56 X0.46
N57 X0.5731 Z-0.7363
N58 G0 Z0.0662
N59 X0.4491
N60 G1 X0.336 Z0.0096 F0.005
N61 Z-0.005
N62 X0.3403
N63 G18 G3 X0.3585 Z-0.0088 R0.0129
N64 G1 X0.3785 Z-0.0188
N65 G3 X0.386 Z-0.0279 R0.0129
N66 G1 Z-0.1297
N67 G3 X0.3785 Z-0.1388 R0.0129
N68 X0.346 Z-0.1541 R0.1341
N69 G1 Z-0.1901
N70 G3 X0.3585 Z-0.1936 R0.0129
N71 G1 X0.3785 Z-0.2036
N72 G3 X0.386 Z-0.2127 R0.0129
N73 G1 Z-0.4454
N74 G3 X0.3785 Z-0.4545 R0.0129
N75 X0.346 Z-0.4698 R0.1341
N76 G1 Z-0.5053
N77 G3 X0.3585 Z-0.5088 R0.0129
N78 G1 X0.3785 Z-0.5188
N79 G3 X0.386 Z-0.5279 R0.0129
N80 G1 Z-0.6329
N81 G3 X0.3785 Z-0.642 R0.0129
N82 X0.336 Z-0.6615 R0.1707
N83 G1 Z-0.7929
N84 X0.398
N85 X0.5111 Z-0.7363
N86 G0 Z0.0466
N87 X0.4596
N88 G1 X0.4491 F0.005
N89 X0.336 Z-0.01
N90 X0.3403
N91 G3 X0.3514 Z-0.0123 R0.0079
N92 G1 X0.3714 Z-0.0223
N93 G3 X0.376 Z-0.0279 R0.0079
N94 G1 Z-0.1297
N95 G3 X0.3714 Z-0.1352 R0.0079
N96 X0.336 Z-0.1517 R0.1422
N97 G1 Z-0.1948
N98 X0.3403
N99 G3 X0.3514 Z-0.1971 R0.0079
N100 G1 X0.3714 Z-0.2071
N101 G3 X0.376 Z-0.2127 R0.0079
N102 G1 Z-0.4454
N103 G3 X0.3714 Z-0.4509 R0.0079
N104 X0.336 Z-0.4674 R0.1422
N105 G1 Z-0.51
N106 X0.3403
N107 G3 X0.3514 Z-0.5123 R0.0079
N108 G1 X0.3714 Z-0.5223
N109 G3 X0.376 Z-0.5279 R0.0079
N110 G1 Z-0.6329
N111 G3 X0.3714 Z-0.6384 R0.0079
N112 X0.336 Z-0.6549 R0.1422
N113 G1 Z-0.6615
N114 X0.4491 Z-0.6049
N115 X0.536
N116 G0 X0.58
N117 Z0.1969
N118 G28 U0.

(PART1)
N119 M1
N120 T1111
N121 G54
N122 G99
N123 G97 S1000 M3
N124 G0 X0.58 Z0.1969
N125 G0 Z-0.795
N126 G1 X-0.008 F0.002
N127 X0.58
N128 G0 Z0.1969

N129 M9
N130 G28 U0. W0.
N131 M30
%

Addtional Quirks

Re: Fanuc 3T Post Processor Needed

George-Roberts — Sun, 13 Mar 2016 19:09:14 GMT

That will be hard coded.. Are you using the generic Fanuc turning post? If so, have you tried changing the type in the properties? The G98 G18 only appears if Type A is selected, see the code below;

  // absolute coordinates and feed per min
  if (properties.type == "A") {
    writeBlock(gFeedModeModal.format(98), gPlaneModal.format(18));
  } else {
    writeBlock(gAbsIncModal.format(90), gFeedModeModal.format(95), gPlaneModal.format(18));
  }

This basically says, if type A is selected, output: G98 G18. If the type is not A, output: G90 G95 G18. Would this be a better fit for your machine?

The following code is what is causing the G28 U0;

  if (insertToolCall || newSpindle || newWorkOffset) {
    // retract to safe plane
    retracted = true;
    writeBlock(gFormat.format(28), "U" + xFormat.format(0)); // retract
    forceXYZ();
  }

This will check if there is a toolchange, new spindle or a new work offset.. If any of that is true, the software forces a retract with G28 U0.

Hope that helps!

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 19:07:26 GMT

What do you mean hard coded?

I am using the Fanuc Turning.cps PP (Generic Turning) I tried some others and it errored out generating the code.

Re: Fanuc 3T Post Processor Needed

Anonymous — Sun, 13 Mar 2016 19:14:15 GMT

So as a new user to Fusion and CNC lathe, Should I keep the G28 U0?

Re: Fanuc 3T Post Processor Needed

George-Roberts — Sun, 13 Mar 2016 20:11:22 GMT

I would keep the G28 U0 if your machine accepts it (I thought all FANUC controlled lathes do). This will move the machine back to its absolute Z0 prior to a tool change.. Last thing you would want is to change tools when your only a couple of mm from the job...
You could probably change it to G53 Z0 if your machine accepts it? Your programming manual should give info on this.

Re: Fanuc 3T Post Processor Needed

scottmoyse — Sun, 13 Mar 2016 20:51:04 GMT

@Anonymous wrote:
So as a new user to Fusion and CNC lathe, Should I keep the G28 U0?

If you are using this as a hobbyist, then keep chipping away and use these forums & tutorials to learn what you need. But if you are running a business and you've just got into CNC, you really should be paying for training.

Have you read through the CNC Handbook? There's a pretty decent page here with links to some handy resources.

Re: Fanuc 3T Post Processor Needed

scottmoyse — Sun, 13 Mar 2016 20:52:56 GMT

Also for Mac's, or any Fusion user, I recommend buying the G-Code editor from cnccookbook.com. Also a great resource for you to get into if you aren't already aware of it.

Re: Fanuc 3T Post Processor Needed

Anonymous — Mon, 14 Mar 2016 02:48:49 GMT

I am still trying to figure out why I cant shut down fusion on my PC?

Everytime I get (Not Responding)

It runs better on my macbook but the menus are different then the PC version and most help and tutorials revolve around PC based.

Yes I have a day job, and my CNC machines are in my home Hobby - Shop which I am tring to desing and make products - So Its sort of a business, just not the one that pays my bills 🙂

Some intersting things happened today, I will be adding a Fanuc 21iT Control to my Stable!!

Re: Fanuc 3T Post Processor Needed

scottmoyse — Mon, 14 Mar 2016 02:59:06 GMT

Maybe look at doing a Clean Uninstall of Fusion, then reinstalling it to see if it starts behaving better on your PC. What are the specs & operating system of your PC?

Re: Fanuc 3T Post Processor Needed

Anonymous — Mon, 14 Mar 2016 03:16:47 GMT

Windows 8

Aspire 5600U

6G System Ram

Intel Core i5-3230M 2.6GHZ

Video Integrated(Intel) Video Outputs Array Intel HD Graphics 4000?

Best I can Find (Been quite sometime since I have even built or looked at computers)

My macbook is a:

2.5GHZ i5

4G Mem 1600Mhz DDR3

Intel HD Graphics 4000

Re: Fanuc 3T Post Processor Needed

scottmoyse — Mon, 14 Mar 2016 03:35:18 GMT

@Anonymous wrote:

Windows 8

Aspire 5600U

6G System Ram

Intel Core i5-3230M 2.6GHZ

Video Integrated(Intel) Video Outputs Array Intel HD Graphics 4000?

Best I can Find (Been quite sometime since I have even built or looked at computers)

My macbook is a:

2.5GHZ i5

4G Mem 1600Mhz DDR3

Intel HD Graphics 4000

Those HD 4000's are probably a bit low spec'd for Fusion. Do they have the latest drivers?

Re: Fanuc 3T Post Processor Needed

Anonymous — Mon, 14 Mar 2016 03:43:28 GMT

Most likely no. I tried to update the PC version earler and encountered an error.

I was needing a new comp anyways was thinking about getting a much better PC based Laptop with 16g Ram SSHD and a Gaming Geforce 960 Card

Ill try to update my graphics card in the meantime

Re: Fanuc 3T Post Processor Needed

Anonymous — Wed, 16 Mar 2016 03:54:46 GMT

Today I noticed the Post Processor both A and B use a G83 for a Deep Drilling Peck Cycle.

My Machine wont support G83 and needs a G74 Cycle. I don't think my machine can use 83 Via Macro as well (85 Miyano BNCT)

Can I modify the PP to use G74 for a full retract peck drill cycle?