Okuma Work Offset - G15 Hxx - Not working?

CGilchrist · 2015-05-27 13:36:05

Hello Everyone,

I just started at a new company that has Vericut. I've got a lot of experience with Vericut on Fanuc controls, but am having trouble with something that should be relatively simple.

I'm trying to get Work Offsets functioning on an Okuma horizontal mill. We use G15 Hxx for the Work Offset. I added a Work Offset table to the G-Code processing, and set the To/From to go From the Tool, to the CSys 'G15H2'. (I created a CSys at the correct location.) When I setup the Work Offset table, it only works if I set the Register value to '1'. How do I get Vericut to recognize that 'H2' is the second work offset value I want to use? When I check in Machine Offsets, it shows Work Offset 1:, as the active Work Offset, even though I'm calling H2.

For Fanuc, I would normally set the Register value to '54' for G54, and my G-code Offset Table; Work Offset entry just maps from the Tool to the correct CSys.

I've already sent the issue to CGTech support, but I'm hoping someone else has ran into this issue. We are just using a "base" Okuma CTL file. Do we need to modify the Control or set some special values somewhere?

Thanks,

Colin

CGilchrist · 2015-05-27 19:42:01

Well, I figured it out. Under G-code Processing > Registers > H* > (G 15), I had to change the 'AdditionalWorkCoord' macro to 'WorkCoordIndex'.

mcam · 2015-06-01 20:24:55

Hey Colin

CGTech have done a ton of work on Okuma controls of late, and I can vouch for that.

Good to see you working with Okumas.

Cheers,

Mike (down in NZ )

oneyankfan1 · 2015-07-07 13:36:45

We have just bought 4ea. Okuma MB5000H horizontals with the OSP300 thinc control. I have always programmed mazaks and used a 3/4 axis fanuc based machine and control file to vericut it with. I know how to use the MCAMV interface and setup tool lists and apply my "generic" 3/4 axis fanuc based machine and control file. That is about the extent of my skill level. My question is how do I make Vericut recognize the G15 HX offset instead of the G54 and the G56 instead of the G43. Is there anything else I should make it do?

CGilchrist · 2015-07-08 20:06:36

I'd recommend starting by creating a Template VCProject file. Just open start a new project in Vericut, then load in your Machine Def and Control Def.

I mentioned in the 2nd post in this thread the one thing I had to change. I had to change the 'AdditionalWorkCoord' macro to 'WorkCoordIndex'. Once I did that, everything worked properly. I'm not sure which version of the Okuma control our Control file started as.

If you look in the "Library" in Vericut, there is an OSP_P200M control. I check that file, and the "WorkCoordIndex" macro is already setup for G15.

So all you should have to do is create a template file that has the Okuma Machine and P200M control selected, and save that to a "template" folder. (Put it wherever it makes sense for you.)

Then when you launch the 'MCAMV' interface, you can pick the Okuma template file, and it will bring in the correct control for you.

(BTW, The OSP_P200M file is also setup to read G56 for Tool Length Comp)

The last part of the puzzle is to make sure you add a Coordinate System (Typically I use the option in MCAMV to setup a Coordinate System that matches my Tool Plane origin.

The one thing you might have to add (either in Vericut itself, or using MCAMV) is a "Gcode offset" table. When you click on "Gcode Offsets" in the project tree, select the "Work Offsets" table in the drop down list, then click "add".

In the "Select from/to locations", you want to set the "From" option to 'Component Origin', and either have Spindle or Tool selected.

Then in the "To" location, select 'CSYS origin'. It will list the CSYS's you have defined in the drop down menu. If you are only using G15 H1, then just select it from the list.

That should be all that is needed for verifying an Okuma program...

oneyankfan1 · 2015-07-31 13:34:44

What if I have 20 offsets (G15 H1 - G15 H20) that run at various locations at various times in the program? Each B rotation has its own offset.

CGilchrist · 2015-08-04 17:30:44

You'll have to setup each of the Work Offset values somewhere. If you know all the numbers to "plug in", you can just create a G-code offset table. For each Offset, you would enter the XYZ and B offset values. Then when the NC file calls up each work offset, it will read the XYZB values from the offset table. The alternative is to setup a CSYS for each offset. You can include the B rotation when you define the CSYS. Then it makes building your Work Offset table easy, because you make an entry for each Register (H1), (H2), ect. These are listed numerically as "Register 1", "Register 2", ect.
Each of these Register entries would be "From" the "Spindle", "To" the "CSYS Origin". (I recommend making each "CSYS" name match your Offset name. (In other words; name each CSYS "G15 H1", "G15 H2", ect.))

oneyankfan1 · 2015-08-24 14:10:45

Im getting everything to work ok except everything at b180 is mirrored in x, the CSYS is in the right spot but its not referencing the orgin when the tool cuts only on b180

oneyankfan1 · 2015-08-24 15:13:58

by the way it might help the response, Im in workpiece view only not simulation

VERICUT Users' Forum

#1 2015-05-27 13:36:05

Okuma Work Offset - G15 Hxx - Not working?

#2 2015-05-27 19:42:01

Re: Okuma Work Offset - G15 Hxx - Not working?

#3 2015-06-01 20:24:55

Re: Okuma Work Offset - G15 Hxx - Not working?

#4 2015-07-07 13:36:45

Re: Okuma Work Offset - G15 Hxx - Not working?

#5 2015-07-08 20:06:36

Re: Okuma Work Offset - G15 Hxx - Not working?

#6 2015-07-31 13:34:44

Re: Okuma Work Offset - G15 Hxx - Not working?

#7 2015-08-04 17:30:44

Re: Okuma Work Offset - G15 Hxx - Not working?

#8 2015-08-24 14:10:45

Re: Okuma Work Offset - G15 Hxx - Not working?

#9 2015-08-24 15:13:58

Re: Okuma Work Offset - G15 Hxx - Not working?

Board footer