Double station vises

[Rory]

We have a VMC set up with 3 double station chick vises.

I would like to know if anyone has any suggestions on what the easiest approach is to program this set up.

I always create the geometry in the first fixture offset. I know that I can Transform the tool path along the X axis, but in order to work on the other side of the vises I cannot transform the transformed tool path by doing a transform rotate.

I would like to avoid creating geometry in each offset because it can become labor intensive to make any changes.

[Guest]

Program the original part using a subprograms for each tool and a fixture offset for each station. With 3 vices and 2 stations each - your machine should have been shipped with G54-G59 to allow for this. Only word of caution is that the orientation of the parts would have to be the same. This will cause the datum to be reversed on half of the stations as the fixed jaw is usually in the middle. As long as you are cautious in the selection of your datums, you should be ok.

Andrew

[Guest]

Forgot to mention that by using subs, the geometry and tool paths are created only once and are easily changed and updated. Documentation now becomes critical for the use and maintenance of revision levels.

[gcode]

At the top of this page is a link labeled

POSTS. one of the posts avaiable there is

the multiple work offsets post. It is ideal

for your application. Set your parameters

(starting G# and number of stations) in

the MISC interger page of the first operation.

[ 08-09-2001: Message edited by: gcode ]

[Rory]

I am trying to avoid the situation that Andrew McRae mentioned, causing the datum to be reversed on half of the stations as the fixed jaw is usually in the middle.

How can I jump over the center jaw and still work with the datum against the center (fixed jaw)?

[ChrisD]

Depending on which machine or control that you have, you may not have to worry about the pieces being reversed on half the stations. In some controls you have the option of rotating your G54 to G59 offsets 180 degrees.

Have you checked to see if this is in your control? If it is, you can have the datum on either side of the fixed jaw.

 

Hope this helps

Chris

[ferdelance]

You should be able to create the first tool path and then rotate it 180 degrees...toolpaths/next menu/transform and then rotate coordinate. You can use a new offset (G54) and your X's and Y's will be inverses. When you set up your stations, the stop point is going to be on opposite sides of the vise for each station. That way you are still using the fixed jaw for a datum. Is that what your asking? That is how we program using multiple work stations with the chick vises.

[Rory]

I understand what ferdelance is saying, this sound like it will work for one vise. How do I work on the next vises? Do i have to create geometry at each vise?

[Guest]

Rory,

The geometry and tool paths will only need to be created on one part. By using subprograms for each tool the same thing will happen at each station. By **rotating**(not mirroring) the datums, the parts will now all have consistant datums - The only problem that I now have is how to rotate the program for the odd numbered offsets - using the convention of even numbered offsets are the three stations closest to the machine column and the odd numbered stations are closest to the operator. What is the control that we are we using here?

Regards,

[Guest]

Again, sorry for the duplicate posts but the objective to maintain associativity of the tool paths and geometry should override the simplified solution put forward through Ferdelance, there is a g-code for a coordinate system rotation on a Fanuc Control but I don't have access to a manual right now. Rory, if you post the gemetry file to the ftp site, I will have a look and see what we can do for you.

Thanks,

[mikee]

For Funac :

G68 rotation on

G69 rotation off

It looks like this in a program

N... M6

...

N... G68 G54 X0 Y0 R0

...

N...G69

N...M6

The g54 can be any work coordinate, and the x0,y0 is the point of rotation in the work coodinate. In this case g54.

R is amount of rotation

Now for the fun. I have always set it up so that at each tool change I turn rotation on ( as needed ) and then turn it off at the beginning of the next tool change. This is because a g53 gets called for tool change.

If you were to change work coodinates without canceling the rotation you could get one big mess.

mikee

[ferdelance]

ok

after you have the first one rotated, then translate both of the originals using transform/coordinate. same principle as rotating but you'll get a different offset for each and your X's and Y's will be the same as the originals.

and since you only have one rotate and one transform operation, you might not have full associativity, but it is a few simple clicks to make changes to the original and then rotate and translate again.

make sense

[ 08-10-2001: Message edited by: ferdelance ]

[Guest]

Rory,

The case that we are looking at here is with a round part. The fist condition where I thought we may run into duplicate datums, just goes away when we have a round part.

Just use the transform and subprograms and the program will acheive our objectives.

Andrew

[Rory]

Its great to have a group like this so we can all pick each others brains.

Thanks much for the help.

Lots of good suggestions.

[toolmann]

RORY,THE BEST WAY TO DO THIS IS IN MASTERCAM.

WHEN YOU PROGRAM A TOOL AND YOU HAVE IT RIGHT.

IN YOUR OPERATIONS MGR. DRAG YOUR OP. DOWN AND COPY AFTER, WHEN THIS IS DONE GO TO THE PARAMETERS OF THAT TOOL AND TURN ON MISC. VALUES, CHOOSE WOORKCOORDINATES AND CHANGE THE NUMBER FROM 2 TO 3 THIS WILL USE G55 FOR THAT VISE AND SO ON. ONCE YOU USE IT YOU WILL LIKE IT VERY MUCH. IT IS A GREAT TOOL TO USE FOR LOTS OF FIXTURES.

[ 08-13-2001: Message edited by: toolmann ]

[Guest]

Toolmann - You are correct that this will work, however to take advantage of the time savings and the power of associativity, the toolpaths/transfrom/translate option is the more elegant solutions with subprogramming techniques.

Andrew

[toolmann]

Andrew that is correct to some degree but when you have operators instead of machinist it is easyer to have one program than many subs, where an operator can make mistakes by strating in the wrong location, as I always say, it is better to spend 15 minutes more at the computer than to have operators make mistakes.

[ 08-13-2001: Message edited by: toolmann ]

[Trevor Bailey]

I certainly agree with Toolmann. We have been cutting a lot of 304 as of late, using Hanita carbide fine roughers. I have programmed everything for subs. The other guy that works with me has never used subs before. It has been a challenge to try and teach him subs, yet alone some other functions of the machine (Fadal) such as simple set ups offsets, etc... You would not beleive how many cutters we have gone thru because of mistakes. I have made everything as "idiot proof" as possible, but sometimes, even that is not enough. Do not get me wrong, my partner in crime is a great guy. He simply comes from a "model shop" only background. As we all know, 3D work is much easier than complex stainless 2d houings with +/- .001 tolerances everywhere. God, what a pain. Give me a 3d part any day.

Trevor

[Guest]

Gentlemen - Ah Finially a good debate over the virtues of Sub Programs! Perhaps NBC can create a new drama based on the forum and have a big name star to rival the West Wing!

Subprograms accomplish the objectives of making each station identical without duplicate geometry or CNC code. It is not the easy way out or the path of least pain. It is a neccessary evil when programming issues must be eliminated during the FMEA and PPAP requirements set forth by a customer. Granted there are a few virgin cutters that will be sacrificed to the gods during the training ramp up, but the end justifies the means. Agreed that this technique is not for everyone but it is possible to stretch the minds of "Operators" and build them into Machinists. As I stated in my second post in this thread. Documentation issues are now of great importance and also as Trevor has indicated "Safe Start Blocks" are essential. I guess I have a case of Fanuc Snobbery as even I would smash the hell out a Fatal Machine... (At least my VIC-20 was in colour! ROTFLMAO).

[ferdelance]

Sub-programs work well when you have operators trained correctly. I use them often. But with the double station vises that are mentioned, you cant just copy the operations and give them a new offset. The work stop must be on opposite sides of the vise to machine the part correctly and keep the fixed jaw as a datum. Otherwise your parts will be mirrors of each other. Which means your X's and Y's are inverses. G68 will fix this problem in the sub-program if that is how you decide to program the parts.

[Guest CNC Apps Guy 1]

I've always preferred subs. It's a much more efficient use of Control Memory. I'm with Andrew. I'm a Fanuc Snob too. They are more expensive to get options for, but sooooooo worth it. Everything is pretty straightforward, and STABLE. Many people do not understand how they work so they tend to shy away from them. Safe restart blocks are mandatory because $%*) happens as we all know.