How to set tools like cincinnati cnc mill

[bigtown]

I started a new job that uses Fanuc controls.

the person teaching me sets all the tools he is using for that job off the top of part.

When I ran a cincinnati mill I set all tools 6" off the table. than you never have to set tools again... Just touch top of part with 1 tool and the machine knows where top of part is and where all the tools in the carousel are in relation to the top of the part.

How can I set the Fanuc so I can set all tools off table and never set them again Like the cincinnati???

Thank you..

[samu]

i'm not sure i understood, if a tool was used for a previous job, he measure it again when he start a new job?? Normally each tool is measured once regardless to the job.

My way to measure tool is to put an offset gage on the top of the vise or directly on the table and with no tool on the spindle i touch the gage with the bottom of spindle, then set relative position to 0. Then i put a tool to measure in the spindle and i touch the gage with the tool tip. Relative position value is the tool lenght that i enter in the tool lenght offset page.

When you set your work offset, you can touch the top of part with any tool and subtract its lenght to the machine coorditate and the result is your Z work offset value.(if the program origin is on top of part)

[chucker]

you can touch all of your tools off the same place in Z then touch 1 tool off the top of the part just like you want to but you will have to put a G54 in your program and when you touch the 1 tool off the top of your part put the number that is in the ABS Z read out in your G54 Z on your work offset page or it can be G54 to G59

[John_B]

I have this situation in my shop. I have one Cincinnati machine and several Fanuc machines.

The Cincinnati has the Seimens A2100 control which is a slightly more intelligent control than most older Fanucs, and it uses a Tram height that is set off of a "standard" block of your choice that sets on the table and the spindle nose is set on, then Tram height set on the control. Then all tools are set off of this same "standard" block and Tool Set selected to create the tool length offset value. Finally any tool is used to set the Z offset by touching to the top of a part and setting the Z offset in the workshift field -tThe control does all the calculations for the tool length being used to arrive at the height of the part in space from the spindle nose at home.

Alot of people don't use a Z offset in the workshift on Fanuc controls, they just set all tools off the top of the part which achieves the same effect a little quicker. This really isn't setting the tool length, it is finding the difference in the tool tip and the part plane. The problem is that it isn't as flexible.

If you use the method of finding the true tool length offset, you need the length from the toolholder gage line to the tip of the cutter. This is normally done off machine using a pre-setter. Then you would need to use a master reference tool holder of some sort to set the Z offset of your G54 workshift or whatever the case is on your machine.

Be careful though. I had tried to get my crew to use the true tool length method on all my machines for a while, but I continually had to retrain them after their getting a small aspect wrong and having wrecked a tool or part. I had to go back to the supposedly fast way on the Fanuc, and continue as normal on the Cincinnati due to operator experience levels. I'll probably try again after I have increased their training levels a bit more though because of the efficiency increase of defining a tool's offset only once in its life.

[samu]

I don't understand the big difference between your cincinatti way of measuring and my fanuc way except that you have somme basic calculation to do with fanuc control. The "fast" way you talk about seems to me to be more complicated and slower!!

[John_B]

Originally Posted by samu I don't understand the big difference between your cincinatti way of measuring and my fanuc way except that you have somme basic calculation to do with fanuc control. The "fast" way you talk about seems to me to be more complicated and slower!!

You are correct, the only difference is the Cincinnati control does the calculations for you so there is no chance for typographical errors (which happens frequently with my operators).

The "fast way" I spoke of is just a dirty way of getting the machine cutting chips, and yes in the long run it is slower but operators often can't see that far ahead to understand the bigger picture. You are exactly correct Samu, your way (the one I prefer as well) is better!

[bigtown]

I want to understand this because it sounds like what I want to do.
Can you explain a little more?

I know years ago people were taught G-code to run CNC machines. Today we are taught to NOT alter the G-code that comes out of the software we use (surfcam,mastercam) or we could crash the machine. So, when you talk about G-code it is hard for me to understand. I have made some pretty complex parts with many shaped pockets and embosses as well as surface contours in Z axis so please don't think I am an idiot, I just don't understand g-code very well.


thank you for taking the time to help..

Originally Posted by chucker you can touch all of your tools off the same place in Z then touch 1 tool off the top of the part just like you want to but you will have to put a G54 in your program and when you touch the 1 tool off the top of your part put the number that is in the ABS Z read out in your G54 Z on your work offset page or it can be G54 to G59

[The Engine Guy]

.
My 2 cents for what it`s worth.
Controls - Seems to work fine on Fanuc OM-Mate (OM-F), Fanuc OM-C, Fanuc OM-B

I spent some time getting the EXACT distance from the GUAGE line of my spindle to the surface of the bed, say -500mm (Sorry, all Metric here!!) for example.

Once I have that figure it will never change unless something pretty drastic is done to the machine, ie bed reground or spindle replaced!!

Then I use the off machine presetting method for all tools and simply input the lengths in the tool offset library, again these never change unless a cutter has to be replaced and then it is only one offset to change!!

Then it is simply a matter of setting the job up in the vice/fixture etc and then I just use a height gauge to measure the height of the workpiece from the bed, if it is for example 100mm then all I need to do is subtract that value from the original total travel amount of 500mm and presto input -400mm in the machine Z work zero and the machine will do the rest!!

Seems a lot when written down but once the initial measuring of the machine and tooling is done then I hardly ever need to make any changes, the tools will always be ready for just about every job, all I usually have to do is set the new X,Y and Z work Zero for the G54 or G55 etc that I am using for that particular job!!

As a "one man band" I find it saves me a lot of time, if I am using for example the same vice/fixture for the next job I only have to measure the height of the workpiece, change the Z work zero, upload the code and press the green button!!

Not saying this is the "right" way but it works fine for me and the info may just be of some use to someone else!!!

It does mean that there is less for the operator to do if you are employing someone, if it`s a problem for the operator how long would it take for you to do the height measure and put the new numbers in yourself?? It`s literally a 5 minute job!!

Do have to make sure with this method that "Top of Part" is ALWAYS Z0 in the CadCAM though, that could get "interesting"!!!!!!

Happy chipping!!

Regards
Rob

.