Origin Offset

[KCollins]

We use a 1/2 inch block to set the tool length offset on all our mill programs. This helps us improve the setup time and not ruin the finish of the parts. I understand that you can change the tool plane origin on every rotation to make the change for the z value on the nc program. Is there a way to make a simple modification to the posts to compensate for this (i.e subtract .5" from the z value of all drill, countour, tap, you name it depths)? As I am continually forgetting to add the offset in the program.

 

If anyone has any ideas please let me know

Thanks

[Trevor Bailey]

Depending on the machine control you are using, why would you not compensate for this in your control?

 

[ 05-17-2002, 12:44 PM: Message edited by: Trevor ]

[Eric S.]

I use a 4" tall tool setter for setting the tool length offsets on our mill. To set the WCO Z height I measure the height of the fixture form the table then subtract the 4" from it (this value is entered into the machines control). This has always worked well for me.

[RandyN]

We use a 4" block off the table also, and set the difference between that and the workpiece in the G54-G59 values as needed.

[Jack K]

I use an 8 inch block to measure my work offset ( 8 inch is easier to grab onto). I measure between the spindle face & work surface then add my 8 inches. All tools are measured outside of machine. Nice & clean works good!

 

jk

[KCollins]

I suggested the same fact. But, I'm relatively new to programming and I was told that it's "just not the way it's done here". I was just curious if there might be a quick switch included in the post but couldn't find one. I guess I'll have to bug my reseller to modify all 40 of our posts...

[Reece L Gibson]

My understanding is that you want Mastercam to add a .5 to all Z movements in the negative direction based on the top of the part being the orgin?

[Verisurf - Ernie Husted]

Hey Randy

 

When are you moving back to California?

 

We have a job opening for you!

 

Ernie Husted

(714) 970-1363

[email protected]

[kathy]

In our shop, for the Mastercam model, we set the Z zero to the print Datum (implied or otherwise). This generally means the top of a bonded panel, or the top of the table for a sheet metal part. Than the numbers in the program correspond to the print numbers. I.e., if the hole is .500 deep, the program code will reflect as: g8_ X_._ Y_._ R_._ Z-.500 … This gives the machinist / operator better documentation so they can know what depth they are trying to make. We found that this mandates the machinist to be responsible for the setup and machined part. When I first started working here, the shop operated more under the conditions you describe. The allowed the operator to close eyes, push button and cry ‘bad program’ when the result was a bad part.

 

The ‘guys’ at the machines use a .010 thk shim under the tools when setting the tools. The .010 is compensated for in the H register at the console, either Fanuc or Fadal. By wiggling the shim underneath the tool, and cranking the dial down .001 at a time, you can get within .001. The shim will protect the material if need be, although it is preferable to set tools to the part off-fall. For critical depth, the machinist will run the tool ‘high’, measure the feature, and ‘sneak up on it’ with multiple passes.

 

Kathy

[Greg Williams]

Hi all,

 

There are many different ways to set the work offsets in the machine, We do it a little differently to the ways mentioned above. We use a block about 100mm, the height of the block is not important, We then measure with an indicator in the machine spindle, using the machine relative co-ordinate system from the Z0 of the job to the top of the block this value goes into G54 Z, All tools in the machine are measured from the home posistion of Z to the top of the block this value goes into the tool length offset. I know that this sounds a little complex and the reason that we do it this way is so that any tool that is in the magazine can be used on any job without changing any tool length offsets. Hope that this helps

[heeler]

We use a process similar to budgie except we have a dummy tool with a .500 tooling ball in it that we use for a base tool. We also use a 3.000" dial XYZ tool setter from lyndex. We then set the dummy tool to the tool setter 0.000 relative and measure the difference to the tools which we put as the tool H offset. You can then set the tool setter to your known Z value, and use the dummy tool to set your G54 ect. Then subtract the 3.000" for the tool XYZ setter. HTH

[Keith Graydon]

We Do it as KathyRic (hi, long time ,no see) describes in her post above. for the same reasons too. Allways from the top Z datum 0. I like using JO blocks rather than shims tho. usually .100". One of our older Monarch VMC's has an auto tool setting routine that really neat.

 

my .02

-KLG