[SQT18MS]

Hi.


We have a Lathe (Alex-Tech Viper 3000 YMS) With the Fanuc 18i-TB controll.

I have problems With setting the tool data for double tool holders.

For the T0800 holder I use T0808 and T0818 for the tool I use in the sub spindle.

But when I am going to set the Zeropoint on the part that is in the sub spindle I can not manually get the T0818 tool to show on the screen.

When I punch in T0818 in MDI I have too reset the machine to get back in manal "JOG" mode, and then the tool data on the screen goes from T0818 to T0800. So therefor I can not set the Zeropoint With the T0818 tool.

Any tips or ideas?

I use G54 in the main spindle and G55 in the sub spindle.

Tha program is a part transfer type, from one spindle to another between operations.

[Heavy_Metal]

Hi,

Check your Fanuc Operator's Manual ( GFZ-63524 ), at page 221.
I think you need the par. 5002 changed, like table 14.1.2.(a), so T0818 means: T08 = Tool 8, 18 = Wear and Geometry no.18
Normally table 14.1.2(b) is selected, T0818 means: T08 = Tool 8 with Geometry, 18 = Wear offset number for tool 8.
Parameter 5002 at page 317 in the Fanuc (GFZ-63539) Parameter Manual.

Regards,
Heavy_Metal
The Netherlands.

[fordav11]

when setting a zero point (i.e. workshift) you should not have any offsets activated in memory. press reset to cancel offsets then move the tool to your zero point and in your workshift screen set the position such as Z0 MEASURE etc.
if your 2nd side is on G55, call up G55 in MDI then set those tools with that workshift active. but you must not call up a tool offset such as T0818 because it will mess up the tool setting and/or workshift calculations when using MEASURE

[SQT18MS]

How do I set the tool offset on the secondary tool in a twin tool fixture if I cant Call up the tool data first?

How would the machine even know what tool is beeing used if they are both in T08.

I will tyr to set the tool offset to a (sub spindle) tool today with manually selecting T0818 when setting the tool offset.

And I will also try to use a single tool holder with no tool (or data on the main spindle side to set the work shift in the sub spindle, and see how that Works out for me.

As I am aware of there are many ways to set up work shift and tool data on a cnc machine, but im not quite sure witch method the previous owner used on this machine.


Im sure with Your help Im going to figure it out.

Thanks for the replies guys

[fordav11]

the machine knows because the geometry is different.
you need to physically set ***geometry*** offset 8 AND ***geometry*** offset 18.

set geometry offset 8 as usual. then on your geometry offset screen move the cursor to 18 and then set the other tool on the right side the normal way. set geometry offset 8 for one side and geometry offset 18 for the other side making sure you are in the correct workshift before you set the tools.
Geometry offset 8 and geometry offset 18 should be different numbers for X and Z. You use wear offset 8 for T0808 and wear offset 18 for T0818.

If you are using a setting arm to set it you may need to disable the auto-cursor selection parameter so you can set the offset numbers yourself manually. Although it should allow you to physically move the cursor position to another tool offset before you set it.

as stated above you may need to change that parameter so the machine reads geometry offset 18 correctly when T8 is called.
I had the same issue on my machine. I would issue T1213 but it would only read geometry offset 12 with wear offset 13 until I changed the parameter. Now it reads geometry offset 13 and wear offset 13 together and I can have 2 different tools at the same T location.

because of the parameter change also bear in mind if you want to use the same physical tool with different wear offsets (for example a ball radius profiling/grooving tool that is capable of being used on both sides) using T0808 on the left side and T0809 on the right side you must make sure that geometry offsets 8 and 9 match exactly. the only difference is the wear offsets in this case because the tool is the same.

[gbowne1]

After installation of my 18iMA after all the components I ordered arrived, I realized this was much easier done than I'm used to on my other FANUCs. Tool and wear pages are easier to read and understand, too. I'm using relatively old software even for the 18iMA/MB. It's the same editions they used in the manual edition.

But I've recently been kinda doin this the same way. Although, I use W&G offsets a lot. Especially since I got the data now. 1 part running a .39" stepover another used a different w the same tool, length, wear, geometry, etc. It's a mix on the same fixtures.