Haas Probing

I have a friend that is looking at a new Hass vf2 and he is thinking about getting the probing routines. I believe he uses Mastercam. What does it take to use the in process inspection and tool breakage routines? Does he need anything special from Renishaw or Mastercam?

Knowing little of Mastercam, unless they gave their own inspection probing, haas is incapable of "easily" inspecting/dumping data. It's primary purpose is wcs probing.

You can go down macro path, or hand editing cam wcs probing routines to generate inspection reports.

Fusion 360 has a newer option that would end up costing around 1700 a year that would streamline the inspection process, but otherwise, macros.

Sent from my SM-G955U using Tapatalk

When you buy a Haas with the probing option included, you get a Renishaw OMP-40 probe, tool setter, and a host of programming options.

On the front end there are interfaces that allow some basic probing for setup. Easy, but limited.

What most folks don't know is that in the backgroud you have all the Renishaw Inspection Plus macros. A most know, these are easily written programs at the control or off-line. Many CAM systems (including Fusion 360) have modules that allow you to more quickly develop these programs, although manually writing them is not difficult. But none of these modules give you the ability to receive probing results back. For that you need something like CNC Reporter.

Mastercam does have a probing module built by Renishaw called Productivity Plus. However, it can be painful to get working, somewhat inconvenient to use, and does not share any of the base macro programming already on the Haas. If a shop has a requirement to produce comprehensive in-process or inspection programs, then the Mastercam solution is worth looking at.

Getting probing data out of a Haas is very easy. On pre-NGC's, its a simple RS232 connection to the PC combined with an application like CNC Reporter to collect the result and put them in reports and spreadsheets. For an NGC, its over the network and also very easy.

Probe guy: not entirely true, on the data reporting. Fusion 360's newish feature "inspection plus" allows users to generate probe measuring macros in cam, run on machine, is exports data back into fusion to give you exact coordinate measurements. It's a fee on top of their standard cam price, but incredibly powerful.

Sent from my SM-G955U using Tapatalk

Agreed...but not what it seems. Fusion 360 (as far as I can tell) does not have a utility that reads the probe results back in and displays them as an SPC-type report. The Renishaw INSP+ software has a built in routine called O9730 which outputs probing results in a text format. This functionality has been in there for 30 years. So, yes, if you just want simple text-only report of nom/act/dev/+tol/-tol, the the standard Renishaw function (which Fusion 360 piggy backs on), will do that. And that would be the same for any CAM utility that post to Renishaw INSP+.

Note that the PC sill needs an application capable of receiving that text report. For RS232 machines, this can normally be handled by your DNC. For NGC's, a file is written to a network folder and can be read by any .txt reader. You need the machine networked and adjust settings 261 and 262.

For someone who would prefer to never hand code a single line of code, I think what fusion has done with inspection plus opens new worlds to users like me, who are quite green to cnc in general (only have a few years experience, first year spent hand coding, but never dipped into macros until recently)

Anyhow, long answer OP, the probe is capable of inspection as long as you are capable of understanding how to program it.

Sent from my SM-G955U using Tapatalk