Avoiding common crash causing mistakes

I am learning to hand code programs. Will move on to cam soon but wanted to learn the basics first. So far I have been running programs first with Z retracted and out of the way. After first cutting air, I run with feeds and rapids down, while hovering over the e stop. I fear screwing up my now running machine. Fanuc Omd.

Anyone have any tips on how to avoid expensive crashes? Or Common mistakes that lead to crashes on a mill?

Thanks, steve.

lowCountryCamo said:

I am learning to hand code programs. Will move on to cam soon but wanted to learn the basics first. So far I have been running programs first with Z retracted and out of the way. After first cutting air, I run with feeds and rapids down, while hovering over the e stop. I fear screwing up my now running machine. Fanuc Omd.

Anyone have any tips on how to avoid expensive crashes? Or Common mistakes that lead to crashes on a mill?

Thanks, steve.

Click to expand...

.
put in single block mode and turn rapids down to 1% and look at the distance to go screen
.
if cutter moving toward table or part at rapid and it says many inches to go beyond collision you
got a problem

Use inc mode when homing

G91G28Z0

G91G28X0Y0
G90

Don't forget to return to Abs mode if that's what your program is in.

All crashes can be avoided by never getting out of bed!

DMF_TomB said:

.
put in single block mode and turn rapids down to 1% and look at the distance to go screen
.
if cutter moving toward table or part at rapid and it says many inches to go beyond collision you
got a problem

Click to expand...

Pretty much this.
Most people don't know how to single block a program properly. Also carry a 6" scale in your front shirt pocket, if you don't wear shirts that have a front pocket.. buy some.
A scale will save your ass more often than you think. Feed hold, look at distance to go, use the scale to make sure.
Learn it, know it, live it.

learn what g and m codes are default when reset button pressed and check screen that list modal
commands in effect
.
keep an eye on G43 and G41 and or or work offset G55 ??

Like Tom said "Distance to go" is your friend when trying things out. I don't always like to run in dry run mode because it normally disables rapid but if your machine can feed really quickly when turned all the way up it could frighten you a bit. I prefer normal Auto mode and rapids just set down really low.

Then a few common mistakes that I have picked up on

- Not checking how high your clamps are and sending a drill or cutter into them. Remember if you are not running high production a bigger "safety rapid plane" is not going to waste too much time.
- As desert said make sure that you are in incremental when homing. As a rule of thumb I ALWAYS go back to absolute right after homing even if my program is using incremental. Turn it on when needed
-Not double checking that all your tool height offsets are in properly (check them... then check them and check them again) It not a problem if the tool is shorter but longer
-NEVER assume that your next line WILL be correct. Remember since you are not using cam and a tried and tested Post your only way to check it is at the machine really. Waste time but rather save your tooling and machine.
-E-STOP is your LAST option... If your rapids are set low while proving programs out your feed hold button in single block mode should be sufficient. I am not saying don't use the e-stop but an endmill digging into a full slot and really going for it might just make you crap your pants more than feed holding and quickly jogging it out of the cut.
-Make sure that Air/Lube/Coolant are all correct. Different machines handle low levels differently. Some might just pause but others could totally switch things off. It truly does suck if you are doing a finishing pass and the machine stops feeding on the wall of a pocket leaving a crappy line all the way up of the wall.
- Make sure that no arseholes are around you to distract you when punching the program in,offsets and proving it out. Distraction is a sure path to you wanting to kick someone in the head. Take if from me as this has happened to me a few times.
-After punching your code in do the same as I said with the offsets Check,check,CHECK. Yeah you will be proving it out but it really is a ball ache when you have proved out 90% of it and have to make a fix right at the end and prove the Whole thing out again
-Most importantly... Be proud of your first few parts no matter how simple they might seem to other. YOU programmed it and set it up. I still smile every time I see the first part come out that I programmed no matter how complex or simple. ENJOY!!! Best of luck!!

Avoid distractions. When doing setups, we post a sign on a stand stating that a setup is in progress and disturbances are not acceptable.

Add 1" to your Z WCS and run the program thru 1" above your part to make sure its doing what you want.

If 1" doesn't get you above your part add more

Sounds like you're on the right track. I like to run programs +6" in Z. That way, at any given point, if I think I have a clearance issue I can stop the machine and stick my 6" scale in between. If it doesn't fit, it's not going to clear.

Some machines, like Haas and Mazatrol, will trace the program out on the screen in edit mode. That's a good way to check if the spindle is going to dive into the table, or something major like that.

On 5x programs, we run everything through Vericut, and that's saved our ass many times. Sound like you've got a little ways to go before you need to worry about that, though.

Don't hover over the E-stop. Use the Rapid and Feed overrides. Set feed to 0% while controlling rapid moves with the override. Then put the rapid override to 0% once you hit a G01. This will prevent the machine from taking off when you're not expecting it.

If you need to hover over something, use the Feed Hold. I'm fairly quick hitting buttons when things go south, but when using Feed Hold only, I've come uncomfortably close to parts in G00.

Single block is purposeful, as is Dry Run (no rapids) and Machine Lock. I use machine lock for tapping cycles, as you can see what the spindle is doing in the absence of Z moves.

i found that with a good cam system you dont really need to run in Z+ at first. but if your really new or dont trust anything it will get you to trust your program more.

obviously keeping rapids down during first runs and setup is the start.

walk in all your tools the first time height offsets are called up. if you have 2 height call ups put an m01 before the next call up so during setup you can stop and walk in the tool again

single block and distance to go is your savior

but i also program in a way that allows me to have the control at the machine. i like to rapid to feed depths with super close leadins but if there is an expensive tool or something special to be cautious of i will initially prog with feeds instead of rapid to z feed, which allows me to single block and slow feed down. then if everything is good ill repost the prog with the better changes once the prog is proved out.

writing codes by hand introduces too much human error to the equation. you should get on that cam asap.

i also will stop the machine at certain critical points and go into handle and jog the machine to the feed depths or other axis moves with very tight clearance etc. its tough to see with coolant and other things going on and alot faster to stop and check before just smashing a tool and then wondering what happened after.

I am glad I asked. All good advice.

When you figger out how to eliminate mistakes post back and let everyone know what you came up with. This equipment used to scare the hell out of me, hand coding you are driving, learn to read the numbers better than the English language. When you get some confidence and think you have this thing dicked is when you really need to be careful. Just do the common sense things to keep you out of trouble and you'll be just fine.


Brent

I was talking to a new operator at ASAP Industries in Houma LA Friday and he told me before he does a new job in his Doosan HBM he manually moves the machine up to the part and sets his rapid limits to .100" from the part. He told me his Journeyman told him to do that as he as well does that too. I am not a CNC operator in any way, shape or form, but as I was watching him set up a part I saw where someone had run a cutter into a angle block on the machine and we were talking about that and he said that. Rich

input data

watch screen on any data you input
.
i thought i typed a -1.0 but machine registered 1.0. and ran a face mill into vise at rapid.
.
sure keyboard needed replacing and it was later replaced. still i should have watched
what i thought i typed. being a inch over part is not going to help if mistake 2" off

Similar to what others have stated, learn to use the distance to go screen. Set your rapids to F0 or 1% (whatever your machine uses).

Use the same clearance plane (example 1") for your hand written programs; which will help you notice something amiss on approach moves.

Set feedrate override to 0%.

That way, when you single block through a program, if the next cycle start begins motion, you will be reminded that you are NOT in linear or circular interpolation mode and need to check your code.

This has saved me several times.

And if your machine has graphics, USE THEM!

Once you get comfortable with your machines and CAM system, you can pretty much run without fear. We more or less just post code and start running. I put in an optional stop at the tool changes so we can check that our tool offsets are correct. We never single block except on the lathe.

ewlsey said:

Once you get comfortable with your machines and CAM system, you can pretty much run without fear. We more or less just post code and start running. I put in an optional stop at the tool changes so we can check that our tool offsets are correct. We never single block except on the lathe.

Click to expand...

Do you draw your toolholders in and your stickouts accurately?
I never have.... I know its capable, but Ive never taken the time to do so. I guess "if" I did, I would be on your level..... but I still 5% rapid from about 1inch down on the first part. Im pretty comfortable with my software, but there are just so many variables in play to just know I have it licked first drop of the gate. Maybe that's where my age and experience come into play.

In my haste I have observed this... I rarely ever fk up a first piece with any other tool that a chamfer tool. Its the tool Im least concerned with for a multitude of reasons, but for some reason, even when I verify etc etc, the chamfering routines are usually where I get bit.

I'll add...

Don't get too "comfortable" or cocky after you have done several successful programs and setups. When I did field service, it was quite common for a new CNC user to go a few months after the install and training with no problems. Then came the call "uh, I had a crash".