VMC Fixture Offset Confusion

[rdoty]

(A followup to my previous posts)

I'm confused as to how to set the XY origin on my material.
Let's say I load a block of material in my vise and run the edge finder up to the LH edge (X). If I'm not supposed to use SETX or SETY how do I record the X or Y edges???? Bear in mind I'm used to my conversational control where I run the edge finder up to an edge and hit SETX or SETY and the display automatically shows 0.0000 for each axis. At that point I hit RUN and walk away.

Then suppose I change jobs and clamp a different size block in my vise. It seems to me that most parts are going to have different XY origin settings.

[SBC Cycle]

Many ways to do it. If you already know the coordinates (including the offset for your edge finder!) you can enter them manually at the command prompt. The format is like this

FO,E#,Xoffset,Yoffset,Zoffset

So if your corner is at X-1., Y2. and you want to use fixture offset 10 you would type

FO,10,-1.,2.

The other method is by using the "automatic" utilities. Type UT in the command prompt (or 1-Setup, 2-Fixture Offsets, 2 read from jog).

First select 1 to establish which offset you want to use, the locater diameter, and the spindle speed you want to use for the edge finder.

When you're done with that, press 2 to jog over and touch your LH edge (don't move it, the control will compensate for your edge finder if you followed step 1!).

When you're there press manual once to return to the utilities.

Now press 3 for store location. It will ask you which axis you want to store; hit X. Then it will ask you which side of the edge your edge finder is on. Hit -

Now just repeat from step 2 above for the Y and you're all set.

You'll notice there are other utilities in there too such as finding the center of a hole using an edge finder. For the dial indicator challenged this is a nice feature and is pretty accurate.

[little bubba]

Also, first space bar menu, #4 "set fixture" will get you to the nice utilities.

The center of a circle is a nice little ute, if I need something dead nuts, I'll use that utility to get a starting center position then come in with the indicator. Most of the time its within a thou or two.

The odd corner utilities are pretty cool too.

[FastFieros]

Originally Posted by rdoty (A followup to my previous posts) I'm confused as to how to set the XY origin on my material. Let's say I load a block of material in my vise and run the edge finder up to the LH edge (X). If I'm not supposed to use SETX or SETY how do I record the X or Y edges???? Bear in mind I'm used to my conversational control where I run the edge finder up to an edge and hit SETX or SETY and the display automatically shows 0.0000 for each axis. At that point I hit RUN and walk away. Then suppose I change jobs and clamp a different size block in my vise. It seems to me that most parts are going to have different XY origin settings.

I ran a Webmatic with a Fanuc 0M controller. The home position was at the end of 2 limit switches in X and Y, and I always zero off the part in some way.

The Fadal has the Machine ZERO also know as CS ... all other points should revolve around this, because PART zero at this moment in time is right now X0 Y0 Z0 also. IF at any point you do a SETX or SETY, you have changed the part zero coordinates.

I do have 'known' offsets. The corner is the location like you describe. Upper LH, outside edge X and Y. Lets say its X5 Y6. That is the offset value I store in fixture offset location 1.

Now here's the question to you. What do you use to make your Gcode? This program needs to be based on either the offset you just set, or you need to know how far it is from the corner of that vise jaw to center of part, or some known location on the part while you are programming in the part.

[donnelson]

if you would like you can call my cell 660-651-9190 on monday and i will walk you through it once you see it done you will see how simple it is call when you can be right at your machine and me at mine
don nelson

[rdoty]

Thanks donnelson, it may be Wed morn. I see you're in KC so that should make it convenient.

[donnelson]

how are you getting along with the exercises

donnelson

[guido5286]

That worked perfect for Xand Y but what about Z? I'm new to Fadal and I'm trying to setup a new part. Any help would be great!

[fizzissist]

...Again, keep hitting the space bar until the page with #6 Offsets comes up. Select it, and from the page that pops up select #4 Utilities.

It will ask you the first tool number, you put in just the number of the tool, hit enter, then it'll prompt for the last tool number, same thing, input the number then hit enter.

It pretty much walks you through the process..where it asks for the height of your block (or what ever you're going to use to tell the computer what the distance is between your program Zero in Z and the tool tip for the measuring process). Then, it'll give you the option of inputting the dia of the tool (which is a good idea if you're going to use the canned cycles that use it or G41/G42),
and then you'll hit the jog button, and move stuff around till you're at the Z height. It says press the Manual button to exit .... go ahead and do it..that retracts the spindle and loads the next tool.

Usually it's best to use an old gage block and move the tip of the tool slightly below it and when the block slides under the tool that's where you hit Manual.
Bringing the tool down onto the block usually damages the tool.

Once you've done that with all the tools, it's a good idea to use Mass Modify to select that same range of tools you just set and input a positive value of whatever your deepest Z move is and add an inch or two for dry run. I write the value on the control, then erase it when I'm done with dry run and reset it back via the same method.