Fanuc post processor, code has lots of errors.

[alonzecustom]

Hi, sorry im new to the forum and im not even sure if iv posted this in the correct place.

G code was generated from fusion 360 fanuc cps post processor.

Machine is a Micro Marco compact 500.

Controller is a M2000w (fanuc compatible)

I will attach some photos of the code and i have written on the lines that are wrong with what we did to correct it.

The same errors repeat all the way through the code.  Is it possible to modify anything so that we dont have to edit the code everytime.

I hope somebody can help us, we are very new to this, its our first machine and are complete beginners.

Thanks Jim.

[engineguy]

@alonzecustom 

Can you upload your Fusion f3d file and attach the Fanuc .cps Post Processor you are using, the code you show doesn`t look right at all, or example at what height does your machine do a tool change? It is normal for most machines to go to it`s Z0 Home position before a toolchange, is it a swing arm or carousel type changer ?

To upload a Fusion f3d file go to:-

File>Export>Select f3d format>Save to a location on your computer>Then attach it to your reply using the "Attachments" facility at the bottom of your reply.

Stay Safe

Regards

Rob

[alonzecustom]

@engineguy 

Hi thanks for the reply,

It is a carousel tool changer, when you do a tool change the z goes to -113.253, the carousel opens comes across grabs the active tool then the z goes up to Z 0. Carousel rotates and the z comes back down to -113.253 to pick the next tool.

I have attached to files you asked for... i think. 

Thanks, Jim.

[engineguy]

@alonzecustom 

Apologies for delay, yes, I had an old Bridgeport that did the toolchange in exactly the same way, the M06 called up the toolchange "Macro" that was burnt into an EPROM an the main board.

Anyway, I have tried to get as close as possible to your images it isn`t exact but may be close so try out the attached .cps file and let us know if it is at all close 🙂 🙂

Stay Safe

Regards

Rob

[alonzecustom]

@engineguy 

Thank you very much it all works perfectly. 

There is just one more thing that its doing that we dont understand, when it does the tapping cycle at the end of the programme the machine stops and comes up with a alarm and its says, INT 011: word data over range.

This is the line of code that it stops on;

G98 G95 G84 x3.81 y-44.45 z-12 R5 P0 F1.

We found that if we change it from a p0 to p1 it will run the code. Only thing is it seams to tap ok on the way in but on the way out of the material it looks like it damages the thread.

Thanks so much for your help.

Thnaks, jim.

[engineguy · Accepted solution]

@alonzecustom 

The P value is the Dwell time setting for when the Tap reaches the bottom of the hole and the spindle has to go into reverse which it doesn`t do instantaneously, it needs a certain amount of time to slow down and speed up again so a lot depends on how your machine is setup, does it have Ridgid Tap, or are you using a "Tension-Compression" Tap adapter or a simple  "Auto Reversing" Tap adapter, for example a Tapmatic, these are great as the spindle only has to go clockwise and as the machine goes up in the Z axis to lift the Tap out the Tapmatic clicks into reverse and  just follows the thread.

Anyway, in Fanuc the P value has a factor of 1,000 so the P1 that you probably put in by hand is actually only 0.001 of a second, a very short amount of time, a thousand of a second, if you go to the "Cycle" tab in your operation and input 1.0 then in your code it will show P1000 or  1 full second, a fairly common setting would be P250 so you would input in the Dwell box 0.25sec, You should have the average Dwell time for the spindle in the machine manual, that`s the place to start 🙂 🙂 🙂

Here is the same hole with a 0.25s value in the Cycle Tab :-

G98 G95 G84 X3.81 Y-3.87 Z-12. R5. P250 F1.

Hope that helps

Stay Safe

Regards

Rob