Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: j2mariashop on May 14, 2020, 12:14:32 PM
-
Fusion 360 just released 4th axis simultaneous machining, which is free until the end of May. I modeled the machining of a camshaft lobe where the lobe rotates on the A axis. However, the post processor file fails as "this post configuration has not been customized for 5-axis simultaneous toolpath". I'm not sure why it asks for a 5 axis tool path, but I'll try to track that down in F360. My question is whether Mach4 is capable of simultaneous A axis (a rotary table on the X axis in my case) machining? I've attached a file showing the error output.
Joe
-
I think I found out what needs to be changed in the Mach4 post process file. In mach4mill.cps, the function onOpen() needs to be modified. The fourth axis is currently disabled (false) and needs to be changed to (true) to activate it. I've attached a screenshot of the edits.
Also see this:
https://knowledge.autodesk.com/support/autodesk-hsm/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-make-a-3-axis-post-processor-from-the-HSM-post-processor-library-support-4-or-5-axis-motion.html
Joe
-
Actually, it still does not work! :-\
The error message from the post config file says "Direction is not supported for machine configuration", "Error at Line 1", where Line 1: Information: COnfiguration: Mach4Mill.
I've attached a file showing the error message. In the code I tested axis direction with a axis:[1] positive direction and a axis [-1] negative direction, but neither seems to work.
Joe
-
Try using a Fanuc postprocessor and see if they have one of those setup for the 4th axis. Then you may be able to adapt what they are doing for the Mach 4 post processor.
Mach 4 is built to emulate a Fanuc 21i control, BTW.
Steve
-
That was a good suggestion. I tried with the Fanuc21i (G91) and it failed with the same error. Must be something I'm doing wrong in the F360 set up. I'll keep you posted.
-
I have the same problem, and spent a day trying different posts, configurations, etc. and still no luck. I suspect this is not supported yet.
-
Go and search on the fusion 360 manufacturing forum
Please read
https://forums.autodesk.com/t5/hsm-post-processor-forum/how-to-set-up-a-4-5-axis-machine-configuration/td-p/6488176
This explains it in detail inc the direction along x or y and WHY
-
Yes, done that - doesn't work. Then the error is about direction... here's my Mach3 onOpen section:
function onOpen() {
if (properties.useRadius) {
maximumCircularSweep = toRad(90); // avoid potential center calculation errors for CNC
}
if (properties.fourthAxisAround != "none") {
var aAxis = createAxis({coordinate:0, table:true, axis:[(properties.fourthAxisAround == "x") ? -1 : 0, (properties.fourthAxisAround == "y") ? -1 : 0, 0], cyclic:true, preference:0});
machineConfiguration = new MachineConfiguration(aAxis);
setMachineConfiguration(machineConfiguration);
optimizeMachineAngles2(1); // map tip mode
}
I also started to look at Youtube videos to learn Javascript so I could program my own, so yes, I did substitute the direct codes, rather than relying on the values in the variables. Same issue. If anyone actually has this working using Mach3 post using the multi axis (not wrap) option, be good to hear!
-
don't shoot the messenger but
here is my mach4 fusion post that works with A along X. I have cut helixes ect with is post but make sure you have Z at the centre of rotation
yes I know its a mach4 PP but they are both based on FANUC same branch
only caveat it outputs a .nc file not tap but mach3 can still read it
in mdi try
G1 G20 x50 a90 f50
that should give you a combined x and a just set z to a safe number
-
Thanks - I will take a look! :D I did try other PPs, and produced some .nc files, which were also errors, not G-Code. I did set z axis as the rotational axis. I will post back if I can get this working.
-
I had high hopes, though there seemed to be no difference in the post Javascript, but no - same issue. Thought I would post some details here of the machine definition, in case that has something to do with it. :(
And the error:
Information: Configuration: Mach4Mill
Information: Vendor: Artsoft
Information: Posting intermediate data to 'C:\Users\User\AppData\Local\Fusion 360 CAM\nc\1001.nc'
Error: Failed to post process. See below for details.
...
Code page changed to '1252 (ANSI - Latin I)'
Start time: Thursday, June 11, 2020 12:00:19 AM
Loading locale from 'c:\users\user\appdata\local\autodesk\webdeploy\production\1f559bb8ae333199306b5c4f1fe680c6eb7ab9e0\applications\cam360\data\posts\common.en.lang'
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.5663.0
Configuration path: c:\users\user\appdata\local\autodesk\webdeploy\production\1f559bb8ae333199306b5c4f1fe680c6eb7ab9e0\applications\cam360\data\posts\mach4mill.cps
Include paths: c:\users\user\appdata\local\autodesk\webdeploy\production\1f559bb8ae333199306b5c4f1fe680c6eb7ab9e0\applications\cam360\data\posts
Configuration modification date: Wednesday, June 10, 2020 11:20:02 PM
Output path: C:\Users\User\AppData\Local\Fusion 360 CAM\nc\1001.nc
Checksum of intermediate NC data: 7720f01aa8be9125834a39cad2271931
Checksum of configuration: 31497b50757641ec0e0985e56b643eb4
Vendor url: http://www.machsupport.com
Legal: Copyright (C) 2012-2020 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.8412
...
###############################################################################
Error: Error: Direction is not supported for machine configuration.
Error at line: 1
Stack dump:
("Direction is not supported for machine configuration.")@:0
onOpen()@c:\users\user\appdata\local\autodesk\webdeploy\production\1f559bb8ae333199306b5c4f1fe680c6eb7ab9e0\applications\cam360\data\posts\mach4mill.cps:220
Failed while processing onOpen().
###############################################################################
Error: Failed to invoke function 'onOpen'.
Error: Failed to invoke 'onOpen' in the post configuration.
Error: Failed to execute configuration.
Stop time: Thursday, June 11, 2020 12:00:19 AM
Post processing failed.
-
Try deleting the machine config from the cam setup
I have had some funny errors using it for 3 axis work , it took a lot of thinking, changing Setting to get it to play nicely
It’s not really needed ,but nice to have when it works save any bo bo,s
-
Good idea, I'll try that.
-
No luck, unfortunately, though the error is different, I've seen it before while testing this 4th axis. It gets beyond the onOpen section, but baulks at a later point:
Information: Configuration: Mach4Mill
Information: Vendor: Artsoft
Information: Posting intermediate data to 'C:\Users\User\Documents\GCode\1001.tap'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Code page changed to '1252 (ANSI - Latin I)'
Start time: Thursday, June 11, 2020 10:35:57 AM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.5663.0
Configuration path: c:\users\user\appdata\roaming\autodesk\fusion 360 cam\posts\mach4mill.cps
Include paths: c:\users\user\appdata\roaming\autodesk\fusion 360 cam\posts
Configuration modification date: Thursday, June 11, 2020 10:30:27 AM
Output path: C:\Users\User\Documents\GCode\1001.tap
Checksum of intermediate NC data: 07209c62a06e8359e0f5498d7bd47548
Checksum of configuration: cc39f4d79fa1ca1e66c5dc12919c75f4
Vendor url: http://www.machsupport.com
Legal: Copyright (C) 2012-2020 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.8412
...
Warning: Work offset has not been specified. Using G54 as WCS.
###############################################################################
Error: Error: Section.getInitialToolAxisABC() is not allowed for section.
Error at line: 1
Error in operation: 'Rotary1'
Stack dump:
("Section.getInitialToolAxisABC() is not allowed for section.")@:0
defineWorkPlane([object Section],true)@c:\users\user\appdata\roaming\autodesk\fusion 360 cam\posts\mach4mill.cps:390
onSection()@c:\users\user\appdata\roaming\autodesk\fusion 360 cam\posts\mach4mill.cps:895
Failed while processing onSection() for record 343.
###############################################################################
Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Thursday, June 11, 2020 10:35:58 AM
Post processing failed.
-
Ok
I have just knocked up a test part
Like a pipe with a flange at each end and a flat lump on the side eg steam cylinder for a beam engine
Axis left end of bed along the x axis
Using that cps I posted it generated code correctly no errors
Z was modelled up from the centre of rotation with x poking out the centre in the normal direction for that axis
The WCS warning was it is looking for a 1 for g54 in the cam setup
So I am afraid you have me stumped, but I will keep my brain cell working ,it’s 73 years old now so a bit slow
Stay safe and well
-
it does work (pokey/mach4) with different post"s
Guess the wcs is setup wrong
-
double check my setup, mmm rotary axis setup X
origin setup wcs but it shows the opposite :)
maybe share your setup
-
Hi, tried setting to mill and turn, but same error. Attached is the setup; maybe something is not right here...
-
ok, this ain't going to work. :) you have to turn the piece 90° aligned to X
look some ytube video how to setup
https://www.youtube.com/watch?v=IPi48a-y0VQ&t=503s
don't select a machine & operating typ: milling just to get going
-
I'll check that one out, but turning it made no difference...
-
OK, I've seen that video - it was made when the rotary was just in Beta, so the setting up is different - and it had a lot of 'quirks' then, as mentioned in the video, and I also had a look at the 'toothpick' video mentioned. None of these provide any assistance with this issue, unfortunately, nor have several others I've looked at, hough none are very recent. It would be good if I could get a simple model sent that works for comparison, perhaps, or I can send mine somehow(?)
-
now setup the wcs: z up & x true the midpoint
-
OK, like the attached? Same issue.
-
& it post :)
-
Really, did you not have to change anything? Can you send the GCode file for it!
-
Hmmm.... maybe I should reboot my PC... you never know. Seems others can get it running no problem.
-
he he, forgot to save it first :)
-
in mach4
double check all 8)
-
Saved it here: https://a360.co/2AZvjHz
Rebooting didn't help, but I guess it must be something to do with my PC if you can produce a GCode (.tap, .nc?) file. Can you send me that? At least then I can machine it.
Thanks,
Barry
-
1:50 in the morning here, have to leave it for later...
-
ok, sleep well :D
https://a360.co/2UzhMNw
-
I've given up on this for now - I haven't seen anyone produce actual GCode as yet, but seems it's possible, so must be a setup issue somewhere on this computer. Might try a different one.
-
think you take the wrong post, better rename the post from stuart. (it has the same name as the standard one)
attached fusion file & gcode it post. (download & open in f360, with the links above seems fusion open existing files)
wcs zero mid/front of the hexagon
(don't machine this, ain't going to look good)
-
look here
two mins work
-
Hi, and thanks for the file. Appreciate the help.
However, it seems the only way I can illustrate the issue is take that file and produce a video capture of my screen, showing that it does not work...I get the same error message when post processing. The youtube link is: https://youtu.be/mVVMVNxgkTM.
It would be really nice if I could get the actual GCode file produced by a post processor, rather than just the model file...
Regards,
Barry
-
Barry
Load that fusion file into fusion use the pp I supplied and generate the gcode your self
Do not play with the settings in fusion except to select the pp
The gcode is to big to post. Anyway I have deleted it now
The pp works .
Fusion works.
It’s the way you are using it , all I did was select the x face in rotation that will be the flat end of the part in the case I uploaded
-
Hi Stuart,
that is exactly what I did - there's one file in the zip, the Fusion 360 file. If you look at the video, you will see two instances of Fusion 360 open - the second one opened with your file when I clicked on it. The video shows in real time I did nothing other than select the default preprocessor (Mach4) and all I get is the error message. I did nothing else! Seems no-one believes it doesn't work, even despite the video evidence!
Also, all my GCode .tap files are small text files, much less than 6Megs (normally a few k, for the most complex).
I don't understand the issue...but thanks for trying.
Regards,
Barry
-
Hi, and thanks for the file. Appreciate the help.
However, it seems the only way I can illustrate the issue is take that file and produce a video capture of my screen, showing that it does not work...I get the same error message when post processing. The youtube link is: https://youtu.be/mVVMVNxgkTM.
It would be really nice if I could get the actual GCode file produced by a post processor, rather than just the model file...
Regards,
Barry
Hi Barry,
When you make your YouTube video 'Private' no one else can view it. :'(
Tweakie.
-
Really? You should be able to use the link, I thought. I'll check into that right now and make it public, if necessary.
Thanks for mentioning it.
-
OK, I set it to 'unlisted'. Will try out the link on a separate PC to check I can see it. https://youtu.be/mVVMVNxgkTM
-
Yes, I can see it on my phone, so should be no problem.
-
Barry
ok looked at your video but even on a 5k 27 iMac I cannot read the error
just for fun as you showed my test cad/cam I have just reposted the code no errors just Gcode
-
Great, thanks. I see your post outputs .nc not .tap, so you are not using the Mach4 post - which one is it you are using?
-
Ah ha! Finally! So I got the generic Fanuc post (not the A axis one that I was using) and put true in for A axis and - yes, it works now! The GCode file helped a lot - thanks to everyone who responded...! ;D
-
I am using the one in post #8. As Stuart.zip
Yes it outputs a .nc file because I altered the post to do that , and yes it’s the one from HSM post lib
It has a few lines altered to alter the patterned behaviour the old code is still there remed out but that will not effect the code for this
Its the one that I did the gcode for you so it works does it not
The mod for the extension in very early on the pp easy to change but you could call it what you like Eg zzz as long as you tel Mach in the config what to look for gcode is a txt file nothing less or more
I will now get some cam done and rest my tired brain cell at 73 it’s old and slow
Glad we helped but
-
:)
-
Hi Stuart, yes I tried your Mach4 post from #8, but that was failing too. The post that worked was the Fanuc one I downloaded from the website.
Thanks and regards,
Barry
-
double check that fanuc post, guess it's 5axis.
the #8 does work fine with the right setup. (pulley turns over X) your setup turns over Z !!! here a 5 axis post ain't going to complain :D
Grts,
-
Dunno about that, Stuart. I got several models from other people here with various directions, none of them worked with the Mach4 one. Might try again, though. I like to find the reasons behind these issues.
-
Ah, found the issue. The process failed because a command (optimizeMachineAngles) needs to be run first before getting the ABC initial axis. Searching for this in Mach4 post, I found that the setting was set to false. Setting this to true, and it now works. :)