[dreamchaser]

I have experience when it comes to setting up mills al day long. but am i supposed to touch the tool off the part and then input the dimensions into the g54,g55,g56 etc... and then input the same numbers into the tool wear offset.

Please help

[fordav11]

the 0i mate may not have multiple workshifts.
usually there is a workshift screen. you touch a tool on the face of the job, move cursor to Z on the left side (Measurement), type 0 then press INPUT.
If you have a MEASURE softkey type Z0 then press MEASURE.

if not like this post some pics of your workshift/offset screens and we can offer specific help.

[sinha_nsit]

After setting work offset (on WORK offset screen), G54 etc., you have to set geometry offset (on GEOMetry offset screen) for each tool: touch the workpiece, type X_ or Z_, with appropriate values, and then press MEASURe soft key. During this process, the cursor should be on the row corresponding to the offset number which you are going to use.
Wear offset is kept zero initially. It is used only to take care of inaccurate dimensions caused by tool wear. When you replace the insert, it is again made zero.

[fordav11]

if you keep your wear offset at zero initially you will surely scrap your part(s).
*initially* the wear offset is set + something for external tools and - something for internal tools. +- 0.010" is enough in most cases, but *rarely* is the offset at 0 even when cutting to true size.

[sinha_nsit]

I do not have enough production experience. So let me understand.
If the geometry offset is set for the correct size, why would zero wear offset scrap the part?

[dak1]

I do not have enough production experience. So let me understand.
If the geometry offset is set for the correct size, why would zero wear offset scrap the part?

It depends on your tolerance. What fordav is telling you is that before you cut, you want to offset your OD tools in the plus direction & ID tools minus. This way, you can make the cuts & have material to recut after measurement if need be. (You can always remove material, you can't add it).

[sinha_nsit]

This makes sense.
But why use wear offset for this purpose?
We can always incorporate this margin in the geometry offset.
With time, when we start getting oversize parts due to tool wear, we can specify the wear value as the difference in the programmed and the obtained dimensions. The advantage is that when we replace the insert, we do not have to enquire about the initial wear value. We would just make it zero!

In my opinion, as an academician, wear offset should be used for the purpose of taking tool wear into account. Afterall, it is supposed to be WEAR offset!

But, as I said, I do not have enough production experience. I always learn from the experience of you people.

[fordav11]

hmmmm, yes indeed. you lack production and machining experience.

when initially setting tools and running a new part you always leave some material on the part for fine adjustment of the sizes. that is done with the wear offset.

even if you set the tool *exactly* with a renishaw probe there will always be a variation in size due to tool pressure and cutting forces. the variation is usually small for external turning tools but push-off on long boring bars can be as much as 0.5mm especially when machining hardened materials or nasty sh*t like inconel. if the tolerance is +-0.01mm and your variation is +-0.05mm you are in trouble.

if you are cutting size then your next part is 0.04mm oversize and your tolerance is +-0.02mm you need to re-run the tool over the part again. if you just run it as-is you will almost certainly cut too much and scrap the part. when re-running tools you add or subtract something to the wear offset to take into consideration the tool push-off cutting forces. a machinist must *always* be aware of how much a tool cuts when re-running a finish pass. the same applies when changing the insert for a new one. a new insert will cut more because it is sharper. so you back-off the tool using the wear offset, take the cut, measure, adjust wear offset then re-run finish pass. then add *something* onto the offset to take into consideration tool pressure when taking a finish cut in one pass (i.e. in production for the remaining parts in the batch). this is where experience comes into play

so basically the wear offset is not only for wear. it is to adjust your cutting size regardless of what affects it.

also the wear offset is easier to change. usually geometry is calculated with MEASURE softkey or via tool pre-setter so the number is mostly minus and large and many people do not understand how it's calculated or where that number comes from so manually adjusting it is dangerous for inexperienced people.
it's far easier and safer to change a wear offset of 0.300 and subtract 0.05 using INPUT+ (which would become 0.25) than to figure out which direction to adjust a geometry offset such as -478.921. the confusion becomes more apparent when you consider that the geometry offset relates to the machine coordinate system and the wear offset relates to the work coordinate system.

[dak1]

It's all good. We all started off with a "lack of experience" in everything!! Time & attention collectively is the means of gaining it.

Either method is workable, but fordav is correct in that the wear offset is much easier & less prone to error than is the geometry. When you offset your cutting path, you are compensating for "process" variations as a whole. You have tool deflection, machine deflection, material deflection, etc... If you take a 0.04 radial DOC finish pass, you'll have different forces than a 0.02 radial DOC finish pass (& different results). A 0.02 radial DOC at 2" dia. will produce different forces than the same 0.02 DOC at 1" dia. The inserts themselves have a tolerance as well so simply starting at zero & going back to zero at insert change may or may NOT produce the required end result (depending on part tolerance). If you're doing tight tolerance parts that you can't afford to scrap as "sacrificial", the process would be to treat an insert change as starting from scratch rather than expecting the same result as the previous insert.

[sinha_nsit]

Thanks Fordav and dak for explaining in so much detail. I have noted that wear offset is not for just wear, and a new insert should be treated as a new insert!

[fordav11]

also note this type of fussing with part sizes is only if you are machining parts with tight tolerances.
if I was roughing sizes without a tolerance or a general limit (for example +-0.010") and needed to change the insert I would just leave the offset alone, change the insert and run the job with the same offset. I'd measure that part and change the offset so the next part would be cutting on-size.

[himatech]

I want to know what is meant by 'T' in geometry/Offset screen I know offset measuring , tool radius and last column 'T' I don't know in Fanuc Oi lathe

[dcoupar]

It is the location of the "virtual tip" that you establish when you touch off your Geometry Offset. On a standard lathe, normally OD tools are 3 and ID tools are 2.

[fordav11]

The T is set to match the orientation of the tool/insert and is used for tool nose radius compensation G41/G42. If you are not using G41/G42 you don't need to put anything in T

[bertus.nl]

the T in geometry/offset means the orientation of the nose radius of the cutting tool .
this is used for radius compensation of the tool

greating bertus