CNC macro programming for probes

Contact Renishaw

Renishaw does not teach what they preach. You will need to do it all on your own. there are plenty of bools on writing macros for milling and turning but, nothing on creative probing practices. I wish someone with this knowledge would step up and write a book to share their knowledge.

I agree with you 100%, I also want to learn the creative macro programming too.

I am having trouble finding the macro books. You would think that you could find them in the book store on the SME website.

The machine tool company will come in to teach for $1200.00 a day.

That is $150/hour.

I need a more econimical way to learn. My company will pay to educate us but there is a limit.

andrecncman,

Not only contacting Renshaw, but also the makers of your CNC centers.

Usually, when you purchase a center, you may have to also purchase certian macros that are already in the machine its just that they have to be turned on. Check the distributor of these machines about it.

If you have a good relationship with your machine tool vendor, they may do it for nothing.

Had operated some Shoda Routers, and we turn on the macros so we could use the probes (Renshaw)

looks something like this; 00101001 .....or was it 101110

After that, you would have to right code (G-code macros) to access these address, basicaly macine location.

good luck,

phoenix911

One of the Machine makers is HAAS, they charge $1200.00 a day.

They claim that they can get me up and running in one or two days.

But I doubt that includes anything other than learning most of the pre-made macros,

not how to modify them or creat my own. I would like to find a more eccomical solution.

On the CNC routers it costed 1500.00 a day plus 2500.00 to just come out. after promises to be out for 3 times, they were a no show. goes to show that throwing money at a problem isn't a solution.

They did have a course from the controllers (Fanuc), which was very useful. It was pricey also. But well worth it.

Those macros include what should already be included but are'nt such as drill pack macros(routines)......G80 and G81.

Each controller is different (even from same manufacturer) Just to know the codes to access the macros. Since you did not buy the units yet, you do have some leverage. AFTER THE PURCHASE YOU LOSE IT.

hope that helps.

We may be creating a cell in one of the other buildings, If so that may be all the leverage I need.

Thanks for your input.

Who is the manufacturer of the controller? Fanuc and Siemens controllers have macro's built in. I'm sure others do as well, I'm just not familiar with them. I have the manuals and I think the macro's for Siemens controllers. Siemens has their manuals online, I'm sure others do as well.

1st step should be to contact the manufacturers of your machines. If the probes came with the machine they will have the info you need. If the probe was purchased separately, contact Renishaw.

Scooter

Are you using CAD/CAM software?

Will it accept a "drop-in" integrated inspection program?

Are you looking to do adaptive machining (adjusting the program to the part) or just on machine inspection (using the machine tool in place of a CMM)?

I never heard of a drop-in inspection program until recently, Renishaw has one for GibbsCam. We are using MasterCam.

Renishaw has a real nice program that you can program off a solid model and watch the probing routines run to check for a crash. You can even open your part program and insert your probing routines. But it cost like $4995.00 and it only comes with one post it cost $1500.00 for each extra post. For 5k it should come with 3 posts. The cost would be more justifyable if it could be applied to more machines. Then what is the training cost to learn the software?

Think about it:

$5000 for the software with one post milling post.

$1500 for a lathe post,

$5000 for a tool setter & probe combo for one machining center.

$5000 for a tool setter & probe combo for one CNC lathe.

$431 for the setting software.

$2500 instalation fees.

$2400 training Mill software

$2400 training Lathe software.

That can easily exceed 22k real fast.

It is no wonder most shops don't have probes or very few of them.

The two main purposes of part probing are setting worik offsets prior to machining or inspection of the finished part while it is still attached to the machine. I would avoid the latter for two reasons: 1, you would be using the same leadscrews and scales for measuring as you do for machining and so any errors in the machine will be carried into the inspection part of the program and, 2, any errors in the calculation of co-ordinates are likely to be repeated for inspection, presuming that the same programmer writes the entire program. For this reason I will assume that you wish to probe prior to machining. This can be as simple as probing one face in order to set an offset, for which the Renishaw software supplied when the probe is installed is adequate, right up to finding the "best fit" for machining a complex casting.

The probe will achieve only one thing - it will send a signal to the CNC controller (eg Fanuc) which will store the position of each axis at the time the signal is received. It is up to you then what you do with this data. The Renishaw manual will tell you where the data is stored, the "Macro Programming" section of the CNC manual will give details of the mathematical and logical operators that can be used in any calculations as well as limits of macro nesting. You will also need to know which of the variables are used by the probe and other macros so that you don't inadvertantly overwrite them in your own program. Having written your macro you should follow the logic through (on paper) using all the possible inputs to ensure that the macro doesn't "fall over" - a macro is a general use program that can be used by anybody for any application and its operation will vary according to the values that are assigned to the variables when the macro is called. Because there is a finite time between the transmission of the probe signal and the processing of that signal by the machine, the machine will continue to move in the search direction and so it is important that the feedrate used for probe calibration is the same as that used for part probing. The Renishaw cycles, which are macros, will ensure that this happens. In order to protect the probe, the machine and the part you will need to capture any errors such as not finding a surface where one is expected, starting a search when the probe is already in contact, variable values not programmed, too many variables programmed, failure of probe to operate properly (no signal, battery run-down, dirty system, etc.) and values outside expected range. If you are intending to write a macro for each application I would suggest that you use a sub-program rather than a macro - it's safer.

To get the most from your probe you will need to have a good understanding of the probe's capabilities and limitations, the data stored when the probe is triggered, the capabilities and limitations of the CNC controller and the machine. Use all the manuals supplied with the machine - the machine operator's manual, programmers manual, the CNC controller manual and the Renishaw manual. A reasonable knowledge of geometry, trigonometry and arithmetic is essential and the ability to think logically would also be beneficial (but, if you are already a programmer, you already have this skill).

I have used a machine probe to obtain "best fit" for a casting, fixing work offsets, setting co-ordinate rotation angles, deciding which program to run, deciding which tools to use, which position in the program to start the run, finding the centre point fron a number of positions (where the usual four points cannot be used) nad, on a multi-pallet machine, by having a "digital" code machined on the corner of each fixture, to probe the fixture code to ensure that the correct program has been selected for that part. The possibilities are seemingly endless.

I hope that this helps you a little but, in the end, it is up to you and your ingenuity.

Yes Thank you very much for your reply.

I have a book from Renishaw but it seem to lack some examples of of ingenuity.

One of my goals is to check to see that the operator has the part loaded correctly, and check location of features before the program starts, and stop if conditions are not right.

But that is a long way off for now, you are right I have a lot to learn.

I did notice that no one in any of the replies said get this book by this author.

You can write a program to check and align your fixturing before a component is loaded - presumably the tooling is bolted to the machine in a nominally known position otherwise you will not have a starting point - you need to know where things are before you can fine-tune the set-up.

When it comes to establishing the accuracy of component loading you would be very unfortunate if there is not some feature on the component that is unique and that should be in only one position. Search for a lump or a hole with the probe and decide whether or not it should be where you find it. For example, if you are looking for a hole you would expect the Renishaw software to return an error "SURFACE NOT FOUND". In your programme, capture this error by setting one of the input addresses so that an error does not occur and then add a conditional branch that depends on the value of the variable that is used for this purpose

e.g. IF #147=1 GOTO 755 (where 755 is the block number that you wish to start from of the condition #147=1 is satisfied)

If, in the above example, the hole is one of two or more holes that are different sizes, then use the probe to measure the hole that you have found and, as a double check, find the another hole and measure that one. Store all your probed data in the CNC variables - this should be done after each use of the probe since the probing software will use the same variables within a limited list set aside for probing every time that a cycle is run: these variables are either cleared or overwritten each time you call up a probing cycle.

Whether you are looking for a particular feature on the component or just checking the position of a face to ensure that the component is located correctly you need to be aware of the tolerances applied to the job before it arrives at your machine so that you do not run into the component before the search begins (Error = "PROBE OPEN") and so that your conditions for acceptance are suitable for the component to be machined. i.e. you don't accept a poor set-up or reject a good one.

Persevere with this one - it will be time well spent and you will find that, not only will your probe become a good friend, but you will quickly begin to ask yourself how you ever managed without one.

One of my goals is to check to see that the operator has the part loaded correctly, and check location of features before the program starts, and stop if conditions are not right.

When I had done it, there was a fair amount of operator input. we used it but not to the extend as I had anticapated.

I did notice that no one in any of the replies said get this book by this author.

When I did do this, this was back in 1991, if there was a book, I did'nt remember, but at the time, I'm sure I wished there was one.

22k or even 50k is not a lot of money for primitive dimensional inspection capabilities. An entry level CMM package is 100K. Understand that "On Machine Inspection" augments more traditional/formal inspection, it doesn't by any means replace it. In my environment we are required to inspect or correlate data on a separate machine, using different software (math algorithms), and preferably written by different programmers before product is released or a die is reworked.

Read, re-read, research and understand the previous post from guest and you will leap forward several years for FREE.

The Mastercam package that you use is partnered with Verisurf, HighRES and Metrolosys for this purpose.