Couple quick questions on probing.

[Anonymous]

Thinking through Fusion probing and have a couple of questions that I have not be able to answer searching the forums.

1. We have hundreds of proven programs that we run often and they generally all use H1 (G54) for the first op so I would not want to have to edit them just to implement Fusion probing. It appears that Probe WCS override can be set to what ever WCS you prefer and then saved as a default value.  So can the probe be set and then reference of of say G59?

2. Once the probe WSC reference is set (assuming it not the same as the part WCS) how to you direct the probe to that new part location? Do you just position the probe near the location the execute the probing routine?

Our post is not yet configured for probing so I can not test its operation so looking for a little guidance from the forum on practical application.

[LibertyMachine]

Ask a dozen machinists how to do something and you will likely get a dozen answers.

I've never used the Probe WCS Override, I've never seen the point. None of the work I do can be loaded so far off location that the probe would fail, so...  ¯\_(ツ)_/¯

Regarding where to probe? I prefer the following mindset:

1) If this is the first op, I will probe a known location, such as center of stock or the hard vise jaw. It's typical of me to program almost everything off of stock centerline, so it's a nonissue.

2) If this is probing for a second op, I would prefer to probe something that's been machined on the 1st op. This isn't always possible, so I'll have one probe cycle to get me close, do some machining so I can reach a good spot and then probe again.

Did this answer your questions?

[Anonymous]

I was asking more on the lines of lets say the last part that was machined was only 1" tall but the next part is 6" tall, How do you tell Fusion that the new part is 5" away (In Z) from the last part?

[LibertyMachine]

Well, some things need to be discussed I suppose.

How do you set up your tool lengths and how do you set up your WCS at the machine?

In my machines, I'm either touching off my tools on a gage block (Mori) or using the toolsetter (Kitamura).

I then establish a Z shift from that point to the top of the part. In probing, I would have this:

T30 M6 (PROBE)

G0 G90 G54 X0 Y0

G43 H30 Z6. T1

G65 P9832 (PROBE ON)

G65 P9810 Z.25 F100.

G65 P9812 X2.0 Z-.3 S1

G65 P9810 Z.25

G65 P9833 (PROBE OFF)

G53 Z0 M19

M1

This would rapid to 6" above the part, turn probe on, protected move down to .25" above the part, probe the width of the part (at Z-.30), update G54, move back to .25 above part, turn off probe and then go home

So, no matter what my part length was, I'm always updating the G54 Z shift. As a job shop, nothing I do is identical to the last job (although the jobs do repeat, thank goodness)

[Anonymous]

All of our machines have part and tool probes.

So are you manually editing the code to insert;

G43 H30 Z6. T1  ?

We run batches of 50-100 parts at a time, several batches a day, so my thought was to output just the probing in one post, for example, Widget-probe.NC, then after the probing then switch to Widget.NC to machine the parts.

[LibertyMachine]

On both machines I do things one of two ways:

1) I post out the entire program (on a new job) with probing and run it start to finish. Probe each piece, every time. Short money.

2) I also have a dozen probing cycles in my machine starting at O8900, each one is a specific probing function;

Width, Single Surface, Bore, Angular etc etc. 

If I'm bringing in a program that doesn't have any probing in it already, I just copy/paste at the machine and adjust to suit.

Are you thinking about doing initial part probing for WCS setting and then just running parts with no probing in between parts?

Do you have a Renishaw probe?

[Anonymous]

Yes, Renishaw probes.

Yes, probe only the initial setup not at the start of every cycle, most of our work has loose enough tolerances to not require probing at each change out.

[LibertyMachine]

Well then! You don't need Fusion for this. Renishaw has another macro program called "Renishaw EasySet" (or some version of that). It's a program with nine macro statements:

%
O8999(REN EZ SET)
M0 
G65P9025A1.D1.1S1. 
(A1. BORE D DIA S OFFSET)
M0 
G65P9025A2.D4.04Z-.4S3 
(A2. BOSS D DIA S OFFSET Z INCR. DEPTH ALWAY MINUS)
M0 
G65P9025A3.Y1.828S3. 
(A3. POCKET X OR Y WIDTH S OFFSET) 
M0 
G65P9025A4.X6.Z-.3S3.
(A4. WEB X OR Y S OFFSET Z INCR. DEPTH ALWAYS MINUS) 
M0 
G65P9025A5.S3X0
(A5. +X TOUCH S OFFSET)
M0
G65P9025A6.S3X0
(A6. -X TOUCH S OFFSET)
M0
G65P9025A7.S3Y0
(A7. +Y TOUCH S OFFSET)
M0 
G65P9025A8.S3Y0
(A8. -Y TOUCH S OFFSET)
M0 
G65P9025A9.S3.Z0.
(A9. Z TOUCH S OFFSET)
M0 
(G54 S1. TO G59 S6.) 
(G54.1P1-G54.1P48=S101-S148) 
 
M01
G0G53Z0
M30

I just go down to the correct line, modify it as needed (width of part, diameter of bore) and run it. Before I run it though, I will bring the probe within .2 of the Z surface, and eyeball it's centrality. It runs this in an incremental mode, so there are zero sudden moves or results such as this:

If you are interested in the rest of the program, PM me your email and I will send it along with more info

[Anonymous]

We have easy set installed, I was hoping to take it to the next level of automation.

Instead of calling up the probe, jogging it into position, selecting the probing cycle, etc it would all be contained into a Fusion probing file for that specific part.

The variable is where to send the probe to find the part to be fully automated.

[Anonymous]

I'm thinking I still maybe able to make this work so I would like to do some testing to try some different approches.

Would anyone be willing to help add probing to my post?

[LibertyMachine]

Adding probing to a post is not a light endeavor, sad to say. My best advice it to form a relationship with a reseller that is experienced in post modification. I've had very good experiences with SilverHawk in Florida

I'm curious how you are going to accomplish what you are looking for. At some point you need to edit fields to give it some idea where the part is and how tall it is..

[Anonymous]

One one of our machines we have 5 double vises mounted on a Sub plate. Normally we run the front of the vises H1 and the rear H2 so we have at a good target to start with.

Probe the part as normal then record the general position such as X-5.2 Y1.6 Z 2.1 on the setup sheet.

Enter the general work offset numbers from the setup sheet prior to running the Fusion probe routines to get the final position.

I may come up with another option but at the moment that is what i'm thinking.