How to stop the G53 at the end of my post - its a darn hassle

[boyd.sofield]

Ive fixed this before and its reappeared again without wanting it. I dont know much about post configurations so I fix this stuff and forget how I did it. The G53 X0 Y0 ZO being posted at the end of my programs has reappeared - can someone please help me out and show me where to remove it?

Ive looked at the normal options in Fusion. Do I need to navigate through my post processor? 

I have changed nothing but its back. I have tried looking everywhere I just want my machine to safe retract and stay where it was. Of course I know I can delete it out of each program but like I say I have fixed it once and its now back. Sorry for being blunt but I get annoyed with unrequested changes. Need some advice please I have a large table on my machine.

[daniel_lyall]

You should be storing your post in the cloud and or your local storage, so every time an update gets done your post does not get over-written.

What post are you useing?

[fritter63]

Hopefully remembering this correctly.... I think I fixed this by creating my own custom post processor, which was a copy of the default one and then I edited out the G53. I store it locally have it set as the default when post processing.

[boyd.sofield]

Hi I am using my cloud version of Mach3 Probing (mim solutions) If I look at editing that, its a massive amount of code. I tried to search for G53 in that and hey, its massive and I know very little about coding. I am sure somewhere I saw a menu option where instead of zeroing the coordinates it just had an option for G53 "safe retract Z" or something. 

I am still looking, and at this time I either delete the line or hit the big red button before my gantry moves 2 meters.

[daniel_lyall]

Attach your post, to have it only doing a G53 Z0, and X and Y stay where they are is quite easy.

[boyd.sofield]

This "pasted below" is the last 10 or so lines out of my code. For some reason its started inserting the G53 G0 X0. Y0. at the end. Sorry I dont understand what you wrote there?

"

X-1.855 Y-2.033
X-2.118 Y-1.757
X-2.18 Y-1.696
X-2.246 Y-1.64
G2 X-2.326 Y-1.359 I0.155 J0.196
G3 X-2.25 Y-0.931 I-1.174 J0.428
G1 Y0.337
G2 X-1.8 Y0.787 I0.45 J0.
G1 G40 X-1.5 Y0.637
G18 G2 X-1.2 Z-20.95 I0. K0.3
G0 Z15.
G17

G53 G0 X0. Y0.
M30

[daniel_lyall]

You need to attach the post you are using so I can show you with your post if it happens again.

[boyd.sofield]

Ok  sorry, I was unsure what you meant. I reckon its not in my post processor its a Fusion thing. Nothing has changed there has been no editing of my post processor. So Fusion either it seems, puts a G28 or a G53 at the end of my post. Totally a pain in the arse tbh. 

Hey so appreciate your help how do I get rid of it? I think attached is what you are asking for to look at?

[daniel_lyall]

Yes, that was it are you sure you used the correct post this one does what you want.

[boyd.sofield]

Hi. Yes absolutely its the same one I have been using for 50+ parts. I just went over my old files and its a few days ago Fusion has started putting the G53 at the end of my programs. Its funny, I get so annoyed with this stuff when its been fine for so long. Looking on the net I am not the only one, seeing there are others with this and some even calling it a fusion bug. Perhaps my version is corrupted or something? I was thinking I will program my system to estop at the end of a program.

[daniel_lyall]

I will have a look in the morning and try with my hobby licences what license do you have?

[Anonymous]

@boyd.sofield 

Is this code what you want?

G3 X12.33 Y-415.509 I0.2 J0.
G1 X12.53
G18 G2 X12.73 Z-7.563 I0. K0.2
G1 Z16.763
G17

G0 G53 Z0
M30

If yes then try changing the onClose area of your PP to look like this :-

function onClose() {
writeln("");

setCoolant(COOLANT_OFF);
writeBlock("G0", "G53", "Z0");   Add this line here
//writeRetract(Z);   Comment out this line by placing the // at the start of the line

//setWorkPlane(new Vector(0, 0, 0)); // reset working plane      Comment out this line by placing the // at the start of the line

//writeRetract(X, Y);     Comment out this line by placing the // at the start of the line

onImpliedCommand(COMMAND_END);
onImpliedCommand(COMMAND_STOP_SPINDLE);
writeBlock(mFormat.format(30)); // stop program, spindle stop, coolant off
if (subprograms.length > 0) {
writeln("");
write(subprograms);
}
}

To get there just use the Edit > Find facility in Visual Studio (Or similar in whatever Editor you use instead) and type in onClose and hit enter and that will take you straight to it, make a copy first and save it in a folder somewhere safe before changing anything. Worth a try, might work for you.

[CaseyChilds]

I've been having this issue as well, and I believe its due to the Safe Retracts option in the post processor menu.   Scroll through the green text menu on the bottom right of the PP box and change the Safe Retracts from G53 to G28.  THe text will turn blue and it reverts back to just retracting in Z.

[Anonymous]

@CaseyChilds 

Different PP, doing your suggestion on the OPs PP gives the result shown below, download the PP that he uploaded and try it out and you will see the difference.

G1 Z16.763
G17

G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

[fritter63]

I think what you're encountering is this (pardon if I do a little mansplaining 🙂 )

When you do "post processing", Fusion will run your CAM setup through a, well,  "post processor" which is a script file (is it in the Python language? I can't remember). This is basically a program script (interpreted language, as opposed to a compiled language such a C++, Java, etc) that reads your CAM configurations and generates your GCode files. 

The default post processor, which I suspect is the one you edited before, was probably recently overwritten by an update to Fusion. This is not a bug, it's how it's designed to work. If you want to customize the script, you must make a copy and save it someplace on your computer (or in the cloud as @daniel_lyall ssuggested). That moves it out of the location where Fusion is assuming it has the right to make updates). You then modify your copy, and the select that copy as your post processor, and it won't get override by software updates, which are now happening automatically even if you don't want them. 🙂

See attached screen capture, note that I have selected "personal posts" as the source for my PP file, and then I selected the one named "Jarvis_...." (because Iron Man rocks). That is simply what I renamed the copied file too. On my system, which is Mac OS, the file resides in ~user/Autodesk/Fusion 360 CAM/posts. Yours may be different if you're on Windoze, etc. Yes, it's a PIA research to figure that out.

Now, the downside of all this, is that if Autodesk makes a GOOD update to the post, you will miss out on that. And of course, they don't let you know that it has changed. Might be worth making notes as to what you've changed, and just periodically checking the version of the default one, then re-editing it to make your changes. What I would prefer to see if some sort of "post processing" hook for the post processor (pardon the overuse of terminology), where I could put in a little bit of script to say "remove this", or better yet, the ability to override JUST the one method that is adding that G53, so that I would still get the rest of the post updates.

Hope this helps.

[daniel_lyall]

@boyd.sofield So far I can only get it to do what you want it to do and if you still are getting the G53 that is strange, I will do the commenting out of the G53 and G28 stuff and post the post back and then you can try it again and it should definitely not add the G53 and G28 stuff.

Try the attached post it should not add the G53 stuff at all, now since it is a dangerous post to start since there is no Z retract at the start do you want one added.

Have you done a reboot of your computer since all this rubbish started happening?

[boyd.sofield]

Hi. Thanks for this. I have tried out the adjusted post and its exactly what I needed. Although I actually thought my post being in my cloud would have kept it from being edited by Fusion? 

If I have read correctly, its in my interests to work out how to edit or adjust the portion of my post processor that inserts the G53 at the end of a program? Yet leave the file in the "system" folder to take advantage of any updates Fusion may want to insert? Actually I have had a proper look and in the different Mach 3 post processor options, there are different options for the safe retract. I am a little confused at why so many.

The Mim solutions post processor is one I have downloaded to support probing in Mach 3/Fusion. Its a large amount of language that is well written (because I am not Jarvis ha) reasonably well explained. Hey would you mind pointing out where you edited it to stop the G53 output?

[daniel_lyall]

---

@boyd.sofield wrote:

Hi. Thanks for this. I have tried out the adjusted post and its exactly what I needed. Although I actually thought my post being in my cloud would have kept it from being edited by Fusion? 

Yes it should have not overwriten it or changed it.

If I have read correctly, its in my interests to work out how to edit or adjust the portion of my post processor that inserts the G53 at the end of a program? Yet leave the file in the "system" folder to take advantage of any updates Fusion may want to insert? Actually I have had a proper look and in the different Mach 3 post processor options, there are different options for the safe retract. I am a little confused at why so many.

Dont leave it in the defult location it will overwrite all what has been added have it in the cloud ar your local storage.

In mach3 you have options to use A G28 or G53 to send the machine back to home when a toolpath is finished you also can have a custom G28 location that you can set there is a G30 option as well, A lot of people dont what this at all you use to have to edite the post to stop this and set a postion for it to goto or have it use the Z move at the end so sending the machine to the Z retract hight solves the issue of the post needing to be edited as all it does is lift Z axis up and stop.

At the moment just use the post as it is in the future the updates to post will not be a problem this is sometime away.

The Mim solutions post processor is one I have downloaded to support probing in Mach 3/Fusion. Its a large amount of language that is well written (because I am not Jarvis ha) reasonably well explained. Hey would you mind pointing out where you edited it to stop the G53 output?

I can do this for you in a vid.

---

Why this happened is a mystery.