Problem- H" as D" offset Fanuc O-M

[CB1973]

Have just purchased a MV-40B and was trying to program a profile then realized that there was no 'D' offset.

Previously on other machines I have always had a 'H' and a 'D' offset

Hence
G40 G80 G91
G0 G28 Z0
G0 G90 G54 X50.0 Y50.0 S1000 M3
G43 Z100. H1 T2 (No problems with the H offset)
Z2.0
G1 G41 D1 X0. Y0.0 (there is no designation for the 'D' offset)

How do I tell machine what the cutter diameter is?

[Chris D]

The H and D addresses are both used to point to the same memory space (offsets).

G43 Z.1 H07

G41 X1.0 D07

In the example above, both blocks would try to use the same offset value stored in offset #7. On controls with shared offset registers, we used to add 30 for tool radius offset storage. With that scheme, the tool length offset registers are the same as the tool numbers. Then for the radius offset storage location, simply add 30 to the tool number.

G43 Z.1 H07

G41 X1.0 D37

Another way to look at is this, in either command you could use either letter (D or H) as they both do the exact same thing - point to a memory location.

Chris

[sinha_nsit]

Offset memory is of 3 types: A, B and C.
C is latest and has both H and D offsets.
A and B usually use H for both length and diameter offsets, using different numbers. H-address with G43 is length offset, and with G41, it is radius offset. Some controls may allow both H and D, but the numbers should be different (in A and B types).

[CB1973]

Clear explanation, thanks Chris.

[gbowne1]

I've been wondering that same thing on my 0M-C.

I programmed a diameter offset for a 4fl carbide SE 1/2" stubby end mill which is actually 0.489" cutting diameter & 0.4985" shank dia held in a CAT40 ER collet chuck with the appropriate collet 1/2". It's a standard length collet chuck but the overall cutting length of the end mill is 1.000". I use this partucular one a lot.
I always have wondered if this is how to do that properly.

I think also I need to rework my work offsets for my Kurt D675 vise. They are not working like I would like them to.

Anyone have any ideas here?

[stevo1]

I use a lot of macros to compensate for different tool sizes or resharpened tools. However if you do not have the macros then cutter comp is the way to adjust for this so you don’t have to change the programmed path to accommodate.

You also have to take into account what Sinha is referring to as what offset type you are using. Offset memory C will have lengthG43H() and offset G41/G42D(). This way you can use the same number for the H and D no need for separate offsets.
T5M6
G43H5Z()
G41D5

Originally Posted by gbowne1 I think also I need to rework my work offsets for my Kurt D675 vise. They are not working like I would like them to. Anyone have any ideas here?

How are the positions of the vises not working for you?? What type of coordinate are you using to position the vise? G54-G59??

Stevo

[gbowne1]

I normally have one or two D675 vises set up with either parts set on paralells, shop made vise fixtures, or on the jaws using locating pins or a work stop. When there are two on the machine table (which is 17x22 btw), I use it to hold long and sometimes long thin parts which get a edge radii.

I am just scared that something might not be set up right and run into something within the work area. I have a really bad habbit of checking for squareness to the X/Y travel on the same parallell as the table especially since the vise sits on a graduated swivel base. 99.99% of everything I do is in inches.

The reason they are not working though is that i have to change everything so much.. and the offsets would be more for some specific parts families that I do.. the actual vise work area needs to be opened up more.

I have and can use cutter comp.. but I use this particular cutter and run these parts so much.. it just would be worth having a macro. it even sits in the first programmed tool pocket.

The stubby is indeed a resharpened end mill cutter, and for now I use it on specific parts. It does use that 0.011" difference in size, just takes off about 0.0055" per. Some time I will go have an actual 0.489 cutter mad but this will work for now.

Greg

[stevo1]

What you need to do is eliminate all of the changes that you are doing. The best way to do this is to setup your machine so that you can offset your tools to a standard and you can adjust different part thick nesses via offsets. This have been discussed many times and everyone has their own way of doing this.

You have tool offsets but do you have G54-G59 work coordinates activated on your control? I will ass u me that you do. First thing is to setup your home position (where the machine goes when G0Z0 is programmed). This is typically off the table face or in your case the vise face. This can be set by using the 1st reference position parameters 708-711 (711 or Z). You can also do this by setting your “common” work coordinate if you don’t want to change the parameters. I prefer the parameter settings.

Now once that is set then offset ALL of your tools off the vise face. At this point if you instate your tool offset and program Z0 the tool tip would go to the vise face. Now all you need is a part height/thickness. Put this in G55-G59. I don’t typically use G54 as this is usually the Fanuc default. Say your part is 3” tall put 3” in G55 Z. Now if you instate your tool and program G55Z0 the tool tip will touch the top of the part. You will never have to touch your tools off again. Just change the Z to accommodate the part that you are putting on the machine.

Stevo

[gbowne1]

I do have G54-G59 activated/enabled. My original home was the center of the vise area (with the jaws wide open and with the vise set in the middle & center of the table and indicated square/trammed. L later chnanged that to the face of the back jaw at the left edge of the vise using a 1/2 dowel pin in a TG100 collet chuck to set it up. The toolchange/set-up home was about 3" away from the table at the outer left end of the table so I could get in there clear of everything to set things up.

My general work area on the vise is generally about 5.125" wide by 3.75" and however deep or high above the jaws.

Yeah I have a lot of changes going on during set up. I have always wanted to be able to emilinate a lot of steps. But then again I am also still learning.

When I first started doing a lot of programming on the 0M-C (and the other controls I have -- 6M-B, 11M, 0T-C, 15M) I was using teach mode. But then I slowly learned all the M and G codes and how to use F, S and T's right from the MDI. I still cant say that I know the specific operation of every one of the codes but I get down and dirty.

Then I got Mastercam 9, and a couple demos of others to try (OneCNC, GibbsCAM and SurfCAM).

I also have been using a vaccumm plate on the mill using a vise to hold the plate and also a tilting sine plate too.

I also would like to be able to do more of what I call "cookie cutter" parts out of thin (.032 to .250) material.

I suppose I will have to change everything when I go purchase a double station vise.

The thickest largest part I do is 12" long by 1.750" thick by 6" wide. It's also the heaviest (C1018). I do a lot of 12" wide by 8" parts on a fixture (one with dowel pin holes and 1/4-20 threaded alternatin set up to locate the part properly.. part rests on pads/buttons.

I would also like to get a little more versatility out of the vise area than I am already.

[stevo1]

So what is taking the time between jobs and what would you like to change??

Stevo

[gbowne1]

The main thing is that takes the most time between jobs, I have so many different fixtures.. that and swithching back and forth between the vise.

The way I have the 0M-C and 11M set up now (both on 3 axis mills) is that I have so many different size parts, different fixtures, and materials. When I finish the 15M machine, it will have a slightly different set up. I just need to figure out how to do jobs more uniformly. Also especially since I'm going into ISO9000/1/2/3 and lean practices

What takes the most time is to make sure that I have everything entered right. Again I do 80% - 95% of my programming right at the CRT/MDI. Then I make sure I have the vise and/or fixture set up. I make careful notes on a setup work sheet on how I do a set up (so I can do it the same way over and over again) and a print of the proven program so if I lose it I can re-enter it. The rest of the time is making sure the toolchanges are done right along with that the tooling in the ATC is right and that i didnt make errors in the program. This is also because I dont have a very good FANUC post-processor.

I also think I overcomplicate my programming.. more so than it needs to be.
I need to be able to utilize G90/G91, G94/G95, G20/G21.. along and add some more macros.. instead of hand coding a lot of stuff.

Greg

[stevo1]

Greg,
There is really no 1 specific way to accomplish what you want but here are a few ideas.

Tooling---As for tools you should never have to touch off your tools for each job. Using gauge line offsets your tool length is your tool length. It never changes so set it once. The only thing that changes is your part/fixture height.

Programs---You should never have to change your program or type it in at the control. The only thing that will make your program different from part to part is your location and tooling. Tooling we fixed so now you just need to locate your part the same way each time. This can be done by using your G54-G59 to set up a specific location of a part that your program is coded around. You should also not have to program or type in at the machine. You machine should have a RS232 port on your machine that you can hook a computer to so you can download the programs when needed.

Fixturing---If you are constantly changing out vises or clamps for jobs there are a few things you can do. You can look at getting a base plate made for the machine so you can put locating pins in that the vises or tooling will butt to so you can locate fast and easy. Going with probes to find fixtures/parts is another option. There are many options here and you will need 1 of 2 things. Creativity or money. Creatively sit back and look at your high running jobs and see what you can do to consolidate your fixtures and tools.

There are so many ways to do this but without being standing in your shoes and looking at your fixtures and parts it is tuff to tell you the best areas to focus on. A lot of the good ideas come with time, experience, trial, and error.

Stevo