Probing WHY AND WHY?

[Anonymous]

Hi guys,

Speaking in terms relevant to my First CNC job (described below)

My question(s) are:

"DOES PROBING ALLOW FOR ANY TIME SAVINGS IN SETTING UP?

"or is Probing just good practice or an extra safe step to include in your Setup?"

Can a Flexicam probe?  If it can, does probing mean, if flexicam doesn't see that part or it isn't where it should be--it will not run the program?  As you can see, I need help from the very bottom rung here : ) but i'm so excited to learn this process.

Note: I am a Brand new user to CNC, to Fusion360, so layman's terms would be extremely appreciated.

My First CNC experience | From what I understand, I am going to want to:

1. secure piece of wood (screw down--we have no clamps) 12" x 6" x 2" the cutting bed

2. pressing a whole bunch of buttons to (A) find the wood, (B) teach it the depth etc. <-- can this be bypassed by probing?

3. then running the program.

but tonight Fusion updated with this magical looking thing called "probing" and am now wondering -- Can I bypass any steps above, by including probing in my program?  How does probing fit in?

(Using a Flexicam http://www.flexicam.com/en/products-en/router-3-axis-en/flexicam-stealth-en.html)

[LibertyMachine]

Probing can be a huge timesaver in running production work, as well as initial setups, once the macros and programs have been established. The probing that has been added to Fusion 360 is based on the system that Renishaw has made, this is also the sytem that is used in Haas machines, if I understand correctly. It's rather unique to each brand of probe mfg, as the system utilizes macros specific to that probe system. If your machine has the option of a probe and it's based on the Renishaw system, then yes, you could incorporate it.

Be warned; An add-in probe system from Renishaw runs in the area of 6-12k, depending on machine and probing unit. I'm SURE there are lesser cost units and methods out there, as accuracy in this case is...relative to the work you are doing. Just not certain how you would go about tying in all the G65 P98xx calls that are currently in the post processor.

CNC tinkering websites, such as those run by the Mach3 community as well as CNCzone might be good places to find out how to bring a low-cost probing system into your machine if the price I mentioned scares you.

[Anonymous]

for Any cnc probing is just closing a input loop . you can find hobby probes from flexcam  it says in that link under measuring. as for the code behind it fusion is moving the machine to a point then running a g31 with variables to tell it what direction to move in , how far and what input pin to look at for a given trip state .

I have seen people run to the ground wire to the workpiece and one to the endmill and set zero with that or use a block with two square sides cut and a thru hole .     

[Stuart-H]

to the OP

search the net there are plans on line to make a 3d probe mine works well and cost £5 and my time which is free to me

have a look at NYCNC on fusion Friday he shows how to do the difficult bit 

OK its hard wired so need to interface to your controler

link if you need it

http://www.homemetalshopclub.org/projects/touch_probe/touch_probe.html

have fun

[daniel_lyall]

@Anonymous what control system does it use of the 4 on the page you linked to. the bottom 3 you will be able to find the codes on line the first one ask them FlexiCAM that is

[Anonymous]

I also don't really understand the point of probing from within Fusion, but maybe it's very specific to the machine in question? My machine has a closed loop servo system. You can hit E-stop, move the table by pushing it by hand, then reset the system and it still knows where it is down to .0005" (resolution of the lead screws) because it never stops receiving positional feedback until you cut all power to the machine completely. It also homes off of the index of the encoders, so even homing is accurate to the resolution of the encoders when resuming work the following day after removing power to the machine.

While I use a probe to locate edges in order to enter work coordinate offsets, I do not see any need to measure/locate edges once the program is underway given that the position of a high end machine is typically closed loop and well maintained from operation to operation as compared to step/dir system where feedback is not supplied to the controller (usually just the servo drives, which make no real corrections to compounding error). Maybe it's for when you locate a new part into a vise for a second operation without a mechanical indexing system? That would seem more time consuming than just creating a mechanically indexed fixture for a production run of anything, so I'd have to guess it may be more useful for one-offs where you are just throwing material in a vise for a second op. I'd really like to hear from people who actually use this feature in order to get a better understanding of what it is useful for.

[xander.luciano]

Hey Guys!

Here's an example where probing is helpful. Say you have a second op part setup in a vice without a part stop. Using a probing operation you can place the stock roughly in the correct position in the vice, probe a known feature, and then machine that part accurately. 

Probing can also be usesful for quickly setting your offset with raw bar stock without having a known part stop on your vice.

I created a tutorial on probing that discusses some advanced use cases for probing.

Best,
Xander Luciano

[LibertyMachine]

In addition to what @xander.luciano mentioned, I'd give you a few example. 

I just finished up this family of small parts. The edge breaks on top and bottom of the hole are .003" max, sharp edge preferred (inspect under 10x magnification). I can profile the part, put the holes in and deburr the top side. Cut it off, flip the part over into softjaws, probe X and Y and deburr the same holes with a .0007" edgebreak all around and it's concentric within .0001 to the existing hole. (And if you are off  more than .0001", it shows up like you wouldn't believe)

Other example: Probing to check the surface to make sure it's where it needs to be. Perhaps the part is moving as you remove a bunch of material. 7075 aluminum is notorious for this. So when you go to finish the part, surfaces aren't quite where they should be. Probing fixes that. I ran a part at my last job that would collapse .004-.007" in length, every time. Do all your roughing and then come in with a probe and establish your offsets again

And my last favorite: Crash protection. If it can be loaded wrong, I promise I will do it at least once. Probing fixes this by using the Skip function (G31 on my machine). Is this hole where it needs to be? What about that chuck wrench, did you forget it in the machine? You can do a lot of "safeties" with a probing system.

[Steinwerks]

Also remember that this is a first step. Even now you could use the post processor to utilize the probe function with specific naming to output your own probing codes without needing more variables. IE call it "PROBE WIDTH" and make that value output specific code related to the relationship of the position. Think in-process inspection. That way if the model changes, your code updates automatically. I haven't delved into this too deeply because I believe it will be coming in not too long a time and this is a logical progression.

Right now I've been hand-coding part flip probe operations and I want to stop! 

Can't wait until it's in HSMWorks.

[LibertyMachine]

Mmhm. It doesn't have probing alignment of a rotary axis, so that's one I'm looking forward to.

Hand coding a probe is annoying, even when you can copy/paste from one program to another. I guess for that matter, hand coding anything is annoying.....

[daniel_lyall]

@LibertyMachine don't you use macro B

[LibertyMachine]

The machine does support it, yes. Truthfully, I do very little with macros, just enough to get by. I know it offers great potential, but eh...I've got software 10 feet from me

[daniel_lyall]

They are very handy if you can use them