[bink]

hi all, long time reader, first time poster. how do i program multiple double vises? we are wanting to put 6 double kurts on the table. we will be drilling, c-sink, and tapping. can anyone help me out? fanuc control. thanks.

[HuFlungDung]

Hi Bink,
The accuracy of the job and the number of work offsets available to you could have an effect. Also, whether you plan to machine all the same parts at all the stations, or different parts at all the stations would be relevant to your decision.

Take a high accuracy job, with one reference edge on the part as the'worst case'. The fixed center jaw is the locator on the vise. Visually, this puts the reference on the foremost edge of the back station but on the rearmost edge of the front station.

This precludes setting a couple of parts in there and running with a simple work offset from one side of the vise to the other, unless you rotate the program 180 degrees when moving across to opposite sides of the vise. This step is necessary to keep the reference edge of the part in exactly the same relative position to the toolpaths in the program.

Now, you might have means via gcodes, to rotate the part program according to which side of the center jaw you are working on. If so, well and good.

If not, then you should make two programs, using your cadcam system to rotate the program for one of the parts. Then, you can run one program, using unique work offsets all along the rearmost stations on all the vises, then switch to the other program to machine with unique work offsets along the foremost station on all the vises.

Now, if your work has a wider tolerance, or has no requirement to accurately locate the parts along an existing edge, then you could simply assign different work offsets to all work stations, and use one program to machine them all. You would write the main program which would contain the calls for a new work offset, then jump to the sub programs which actually contain all the toolpath code.

Do you want to use one tool at all stations, or do you want to machine complete, but different parts at all stations?

[Geof]

hi all, long time reader, first time poster. how do i program multiple double vises? we are wanting to put 6 double kurts on the table. we will be drilling, c-sink, and tapping. can anyone help me out? fanuc control. thanks.

One way to do this is to make your part program into a subroutine in what becomes a coordinate definition program (if your machine controller will handle subroutines). Then you define a work zero for the center of each vise which gives you six work zeroes, or a work zero for each part which gives you twelve works zeroes. Your coordinate definition program then sets each work zero and then calls the subroutine. Something like this:

blah
blah
G54 M97 P1000
G55 M97 P1000
blah
blah
M30
N1000 (Part Program)
blah
blah
M99

Your machine may use something different to M97 P1000 to call the subroutine; these are the Haas commands.

A disadvantage to this method is you have to enter a lot of work coordinate numbers so another way is to use G52 and you only need to enter coordinates in the program when it is written...but if the vises are removed you have to put them back in the same place or edit the program coordinates. The program using G52 is:

blah
blah
G54
G52 Xfirst Yfirst M97 P1000
G52 Xsecond Ysecond M97 P1000
blah
blah
G52 X0.0 Y0.0
M30
N1000 (Part Program)
blah
blah
M99

Your machine probably uses G54 as default. If you do not put anything in for G54 then it is at the machine home position and you simply need to find out the first, second, etc, X and Y coordinates which will be the same values as you would have used for the individual work zeroes.

Both these methods with the entire part program in a single subroutine finish one part at a time so there is not much benefit to having multiple vises because you do not reduce the number of tool changes.

To have one tool change for every twelve parts and speed up cycle times you put each tool in its own subroutine. Then you select the work zero by either method, multiple G's or G52 then go to the tool subroutine. Your structure then becomes:

blah
blah
G54
G52 Xfirst Yfirst M97 P1000
G52 Xsecond Ysecond M97 P1000
G52 Xfirst Yfirst M97 P2000
G52 Xsecond Ysecond M97 P2000
blah
blah
G52 X0.0 Y0.0
M30
N1000 (Tool 1 Program)
blah
blah
M99
N2000 (Tool 2 Program)
blah
blah
M99

All of this is assuming you are doing identical parts at each location. For different parts which may use some of the same tools you simply have two tool subroutines; N1000 for one part, N1100 for the other and you have the tool selection in the subroutine.

[solgood]

Not sure if this is a option for you, but if u plan on using these vices allot for this job and others i would machine the vices and table for repeat setup.

First look on the bottom of your vices there should be two blind holes (one in front one in back on center) ment to hold slip fit dowls and two taped holes (one on left and one on right on center) these are ment to hold key stock. I dont know if Kurt does this or not, i work with Chick vices so if they dont just machine them your self.

After u do that mill a key way across the center of your table to mesh with the keys on the bottom of the vices. Then drill and ream slip fit blind holes in there proper locations.

Then put dowl pin in the reamed holes on your table and set your vices over them. Bump them back and clamp down.

Your work zero for x is the left edge of the fare left vice and y is the center of all vices. So u are always working in x positive and y neg. is the front jaws and y pos. is the rear jaws.

After u set up for the first time there will be no need to indicate and edge find. Realy fast setup.

Let me know if u have questions

[solgood]

I would drill and ream the vices and the table for slip fit dowls. Then drill and tap for key stock on the bottom of vices. Then mill a key way across the table.

work zero x= left edge of far left center jaw and y= center of all center jaws.

no need to ever edge find or indicate after first setup.

let me know if u have questions

[Geof]

Not sure if this is a option for you, but if u plan on using these vices allot for this job and others i would machine the vices and table for repeat setup...I dont know if Kurt does this or not...

Kurt vise do have the key slots and holes. We mount ours on subplates which are keyed to the slots in the machine table. Just makes it easier and quicker to switch the vises in and out.

[HuFlungDung]

Keep an eye on Ebay for subplates. (Auction gloat follows ) I needed to extend my table top area on my Haas VF3, so I could hang a large rotary table off the right end and still have 40" of useful machining area. Weellll...... it so happened about that time, a 20 x 50" Bock came up on Ebay, and....what can I say......I stole it! $500, and it came with all the hole plugs and everything. I still have not geared it up to hold a bunch of vises, but one of these days, the right job will come along and force me to advance

[bink]

We are definitely gonna make pins for the vises.

I am going to use subs for each tool, and we want to drill all the parts, then c-sink all the parts, then tap all the parts. so to use the g52 command, do i set g54 at the middle of the center jaw for y, and the left edge for x? then edge find over to the parts to get the #'s and plug them into the g52? would it be best to start in the front jaw of the vises and then work left to right, then move to the back jaws, then work right to left, or just completely do the first vise then move to the second vise and so on? anyway, so if it was 2" in x and y:
(From the front jaw of the 1st vise #1)
g54
g52 x2.y2. m98 p1005 (drill sub)
g55
g52x2.y2. m98 p1005
g56
g52 x2.y2. m98 p1005
etc.... to g59
then (now i'm on the back jaw of the far right vise #6)
g59
g52x2.y-2. m98 p1005
g58
g52x2.y-2. m98 p1005

[Geof]

I think the way I described it was a bit confusing. I intended to mean that you can do it with a whole bunch of work zeroes G54 through G59, or using one main work zero and a bunch of subsidiary work zeroes defined by G52, but not both combined.

I should ask the question have you used G52 before; I find some people use it all the time but some people have never used it. Perhaps you can post a drawing of the part and hole layout and where you put you work zero now and I can possibly give some idea how I would try setting things up. We do this all the time for our products and it is really easy to decribe standing in front of the machine waving your arms around. Trying to doing it in writing is real difficult because you can't see the arm waving.

[bink]

thanks geof. i haven't used g52 before. the part is 1.25 " dia., and 3.25" lg., 3/4-10 tapped hole in the center. the vise stops are just screwed into the vise jaws. could you explain the g52?

thanks

[bink]

sounds like all my g52's come off of my g54. then cancel the g52 in my main program........

[Geof]

sounds like all my g52's come off of my g54. then cancel the g52 in my main program........

Yes.

You have six vices that can hold twelve parts which means that to use G54, G55, etc, every time you do a setup you have to enter all these work coordinate values into your machine.

With G52 all these coordinates are in your program as the X and Y in the twelve G52 statements.

You have to find out what the coordinates are either way and you have to make sure the vises stay at the same spacing for G52. Your first setup for the job takes the same time whichever way you do it but your second setup only requires entering G54 because everything else is now in the program.

I mentioned putting the vises on a subplate. When you do this the vise spacing is fixed and you can machine a reference hole in the subplate and then this is the location of your G54. The subplate needs keys to line it up to the machine table to keep it parallel but the sideways position does not matter if the reference position is on the subplate.

How many parts are you doing? It sounds like you are doing lots of these if the purchase of six double lock vises is justified; I just bought three Kurts and they are not cheap. Are you using custom jaws so you can clamp two parts per jaw set for a total of 24 parts per load?

[shawnc74361]

I machine 12 parts at a time very similer to what you are talking about. I use macros to load the work cordinates as folows

T1 M6
S12000 M03
M98 P7001
G00 G43 Z.1 H01 M07
G54 P101
M98 P101
G55 X0 X0
M98 P101
G56 XO YO
'' ''
ALL THE WAY TO G59
THEN IT GOES
M98 P7002
G54 X0 Y0
AND SO ON

The 7001 and 7002 and so on are marcos the load the x, y, z, into the g53,g54, g55,g56,g57,g58 ,g59 the g53 is important it is the master and g54 through g59 is incramintal from g53. I dont have a sample right in front of me on the 7001 subs but it is fairly simple to use once you see them. I have 5 machines that use this program style it runs great. I set all my tools in a master location and have the programs all set and stored. All my vises use quick change jurgens pins. I can litterally up load a program, change vises and be running a totaly different part in less then 10 min. All my parts use standerd tooling, all the machines have the same tooling and have 40 tool turrets. All tools stay in the machine its a snap. I will post a sample of the macro tomarrow.