Checking CNC Programmes

Checking CNC Programmes

Category : Beginners

Checking CNC Programmes (Prove-Out) Without Tears

I am always amazed when I watch people Checking CNC Programs or proving out as it is sometimes known.

Even experienced machinists with years of experience often do this completely wrong. It really can be done without crashing the machine.

Checking CNC Programmes

What You MUST NOT DO When Checking CNC Programs

  • Don’t allow anyone to stand over you especially if it makes you nervous tell the boss to piss off.
  • Never ever rush this process.
  • Always carry out all the checks below before you prove out.
  • Don’t cut corners.
  • Never take off machine interlocks or override any kind of safety device.

Have a Plan

It sounds stupid but what will you do if something goes wrong when you’re Checking CNC Programs.

Do you remember when you first drove a car? The first emergency stop you did? Well you didn’t automatically hit the brakes and depress the clutch did you. You had to think.

When you are an experienced driver, in an emergency you will automatically  hit the brakes. This is because a path is permanently etched on your brain and it’s almost an involuntary action.

This is the same with a CNC Machine if you are used to hitting the E Stop button then it will come automatically.

If you are like me, working on lots of different CNC Machines almost everyday, then you really don’t have a clue where the Emergency Stop Button is.

The Plan For Checking CNC Programs

It’s easy, if you are new to the machine and you have any doubts at all, hold your hand over the Emergency Stop Button. Then in your mind think “one false move and you get it sucker”.

Pressing the E Stop button doesn’t start world war three but what it will do is halt everything instantly.

Yes you will have to go through your machines start-up procedure. You may have to get a boring bar out of a tight spot but you didn’t break anything did you. That’s the idea.

So to use the car analogy. You think…..
  1. Press brake and clutch.
  2. Control the car.
  3. Panic (it’s OK now you didn’t kill anyone)
So do the same with your machine…
  1. Press the Emergency Stop.
  2. Mmm, there is no number 2

Obviously your plan will not always be to hit the E Stop. This would be a very short blog if that’s my only advise.

Checking CNC Programmes

You may just want to press Cycle Stop or the Feed Hold button. The main idea is that you are covering the button you’re about to press. This keeps things really simple, the way I like it. In a panic you won’t have a clue where the button is.

The System When Checking CNC Programs

When Checking CNC Programs (proving a program) you should either be looking at the program with the machine stopped or, looking in the machine whilst it is running. You can’t do both at the same time so….

  • Stop the machine and look at the program.
  • Start the machine while you’re looking inside with your finger ready to feed hold or E stop.

Dry Run

Most machines have a Dry Run Button or switch. Personally I never use them. Dry Run gives you a feed control over both rapid and feed moves and it does depend on parameter settings as to how it works.

It means that you can control all your moves with the feedrate potentiometer.

Sorry for being posh a potentiometer is the dial thingamajig. Say it in front of the boss and if you get a pay rise I want a percentage.

Checking CNC Programmes

Anyway try it and see what you think, (dry run that is). Your machine parameters will give you the option to override rapid moves or not.

OK so why don’t I like it? That’s an easy one. It is easy to get carried away and feed really fast on a rapid move but don’t forget when you come to the next feed move you are probably feeding way to fast and you will break the tool.

Yes you have guessed it I have done that on a few occasions.

On some controls Dry Run will stop the spindle from running so it has to be run in fresh air with no part in the machine.

Rapid Override

Buttons or dials, you can override all rapid moves by a percentage.

Checking CNC Programmes

On the Heidenhain control panel the override works for rapid and feed moves so you just have one control.
Checking CNC Programmes

Beware because some controls have a massive difference between the slowest and the next setting. It’s either like watching paint dry or shit off a stick.

Checking CNC Programmes

Machine Lock

You can use the machine lock which does as it says. Nothing moves so it is purely for testing the code. All the positions etc will change so you will see everything moving on your position display but the axis are locked.

CAUTION

On some older machines the machine will completely lose its position and you will need to zero return after using this.

MST Lock

If you use this let me know cos I don’t know anyone who does. It effectively locks all M Codes all S Codes and all T codes.

So:

  • No coolant.
  • No spindle start.
  • No tool change.
  • Etc Etc

Running The Program 10 Foot Above the Part

Again not something I do. Some people like to run the program above the job (in fresh air). Or on a lathe away from the chuck.

The only problem is you still won’t be sure the program is OK when you do it for real. Anyway do it if you want I won’t ban you from my website or anything.

Graphics

If you got em use em. A lot of, in fact all machine graphics tend to be complete dogshit.

It is not like a CAM system such as Edgecam where you can completely collision check your program.

Don’t forget it’s a good way to pick up coding errors and you will see if you drilled a hole miles out of position.

We are looking for the big hitters here, big mistakes.

Checking CNC Programmes

You definitely won’t know if a hole is a mm out of position but that is not really the idea. Read this article.

The Dangerous Bits When Checking CNC Programs

The most dangerous part in any program is when each tool first comes down to the part.

Why?

Because that’s when you apply the tool length and the work offset. Both of these can be wrong.

The second most dangerous time is when the tool leaves the part and goes back to tool change position.

Before You Start, Be Patient Tiger

Let’s do a checklist Before Checking CNC Programs Out
Milling First.
  1. Check datum in MDI. Move your machine to X0 Y0 in your work offset as a test.
  2. Does every tool have its length set? If you use proper tool lengths then you can manually measure each tool with a steel rule as it comes out.
  3. All tools needing G41 G42 compensation will need their radius or diameter setting in the offset file. (Here is a video on G41 G42 if you are unsure)
  4. On Fanuc type controls make sure the T and H codes correspond. On a Haas Machine this can be automatically checked by changing a setting and it will give an alarm.
  5. Also on Fanuc type controls make sure your D offsets are correct.
  6. Check the first movement line of each tool it should contain G90 absolute and the Work offset.
  7. Try to always make your programming format the same. That way you will easily spot mistakes. Read this article on well set out CNC Code
  8.  Learn about modal G codes. Make sure the first feed move has a G01.
  9. Clean all your internal guards make sure you have the best view possible.
    Now Turning.
    1. Check work offset in MDI send a tool to Z0.
    2. Does every tool have its X and Z offsets set?
    3. All tools needing G41 G42 compensation will need their radius and virtual nose position set. (Here is a video on G41 G42 if you are unsure)
    4. Check your tool change position is adequate to clear every tool. A sub-programme is useful for storing this as you only need to get it right once. And don’t forget that turret will spin around here.
    5. Remove long large tool if not in use.
    6. Check that each tool calls its offset T0101 (Tool one offset one).
    7. Check the first movement line of each tool.
    8. Try to always make your programming format the same. That way you will easily spot mistakes. Read this article on well set out CNC Code
    9.  Learn about modal G codes. Make sure the first feed move has a G01.
    10. Make sure you have a G50 speed clamp. Read this article to see what happened when I missed it out.
    11. Clean all your internal guards make sure you have the best view possible.

Here’s A Thought

If your rapid is nice n slow even if you hit the part with the tool as it approaches the workpiece.

  1. I probably won’t break the tool.
  2. If it cuts the metal, so what.
  3. You will have time to stop it.
  4. You probably wont get fired.

How we Teach Checking CNC Programs (Prove Out) at The CNC Training Centre

  • You might want to reduce spindle speed for the prove out.
  • I don’t start the spindle until the tool gets to the workpiece. That way there is a lot less drama.
  • Set rapid override to minimum.
  • Set position screen so that you can see the distance to go or remain. You must be able to read the program (a printout may be useful).
  • You need to be able to view the modal G codes as well as spindle RPM. All controls will have a screen to show this along with loads more useful shit.
  • If you have a set-up key then use it. It will allow you to do more things such as opening the door at low RPM.
  • Check your manual to know exactly what you can and can’t do when you stop your program. This varies massively between machine tools.
  • Set your Optional Stop switch or button to on. If you have M01 before or after each tool then the machine will stop.
  • Set single block to on. This is a button or switch. This means for each block of code  (line ending in ;), the machine will read it, do it and wait.

 

Checking CNC Programs

So here we go…..

  1. Rewind and Reset the program to the beginning.
  2. Press cycle start as you look into the machine. Be ready to press Feed Hold or Program Stop button.
  3. If your rapid is set nice and slow it’s OK to switch off single block until the machine starts to move. As soon as it does press Feed Hold and turn Single Block back on. This may be necessary if your tool change program (which is not normally visible) allows single block. This means just a tool change will require loads and loads of presses of the button.
  4. Watch as the tool gets closer to the workpiece. Press feed hold when it is close to the workpiece. (It may stop before this).
  5. Now read the program.
  6. Look at the remaining distance to go. If this is a massive number it’s time to panic.
  7. Now work through each block like this.
  8. Stop the machine and look at the program. Read the position display. Start the machine while you’re looking inside with your finger ready to feed hold or E stop.
  9. When you have completed the Prove Out run the program without single block but still keep the rapid nice and slow.
  10. After a few parts you can put rapids up to maximum.

Remember when the machine is moving you should be watching not looking at the display. Only look at the display when the machine is stopped.

I could say good luck but I would never expect you to rely on luck. Be patient and follow the above and you wont need it. As Louis Pasteur said luck favors the prepared mind.

Thanks for reading this article and don’t forget the most important thing is your personal safety and the safety of others.

Services offered at CNC Training Centre

Edgecam Training.

Classroom programmer training.

Onsite CNC Machine Training.

CNC Training on all controls and machines.

Mazak Training Fanuc Training

Don’t forget we offer training on all types of Mazak Machines and all Fanuc Controls 6m to 31i Oi old to young.


Log out of this account

Leave a Reply

CNC Training Centre
WP to LinkedIn Auto Publish Powered By : XYZScripts.com