G0G91G28Z0. cancelling G43 offset

markgerke · Jul 30, 2021

Hello,

We have a Fanuc Oi-MF control on an Awea AV1000 mill.

If G43 H4 is active for the tool length offset and I do a G0G91G28Z0 or if I do G0G91G30Z0 the H4 value is cancelled.

If you look at the position check screen where you can see all active G-codes and H & T values it still shows the H4 as being active but it is definitely not active anymore after the machine returns to zero return or 2nd zero return.

I am fairly certain this is a parameter issue. If someone can tell me the parameter to change it would be greatly appreciated.

Thanks!

Ox · Jul 30, 2021

This app is only barely in my wheelhouse, but when you punch in G28, that runs off of "Machine Zero" or whatnot.
It has to dump any tool, fixture, or G10 offsets to make this move.

Now - you say that it is still showing active in your list, and if so - then it only disregarded it for the G28 move, but maybe it is still active should you want to continue for some reason from a G28 position - although that seems an odd application.

What is it that you are expecting - or desire it to doo differently?

--------------

Think Snow Eh!
Ox

13engines · Jul 30, 2021

Not sure why you're running home and then back again with the same tool, unless there's some in program clearance you're after. Your problem might be that I don't see a G90 mentioned after all your G91 activity. Perhaps your machine is returning to work under an Incremental mindset.

Another route is use G53 instead of G28. Simpler way to obtain the same movements, and it won't take you out of Absolute Mode.

angelw · Jul 30, 2021

13engines said:
Another route is use G53 instead of G28. Simpler way to obtain the same movements, and it won't take you out of Absolute Mode.

The Tool Length Offset is also cancelled by G53.

@markgerke
Check carefully that the Tool Length Offset is still active with the next Z Move in Absolute Mode, as it should be restored.

Regards,

Bill

Booze Daily · Jul 30, 2021

Check to see if G49 is active. That's what cancels tool offset.
The H value would be the last H value read.

If you called G43 with no H, it would use the active H (in your case H4)

angelw · Jul 30, 2021

Booze Daily said:
Check to see if G49 is active. That's what cancels tool offset.
The H value would be the last H value read.

If you called G43 with no H, it would use the active H (in your case H4)

Hello BD,
Not necessarily, it depends on the setting of parameter bit 5001.2. If set to "0", that's correct. If set to "1", then Offset H00 will be made active, which is the same as cancelling the Offset as H00 has the value Zero and can't be set otherwise.

Regards,

Bill

srp61 · Jul 31, 2021

So, I've always wondered why Fanuc(and simaler) use separate diameter/length offsets.

Is there a practical reason or is is some legacy thing from older controls.

I'm sure there's a good reason I just can't think of one.
(So I'm coming from Heidenhain where the tool call contains all the info and tool lengths aren't cancelled (well I suppose they are temporarily)
by moving in machine coords etc)

Ox · Jul 31, 2021

srp61 said:
So, I've always wondered why Fanuc(and simaler) use separate diameter/length offsets.

Is there a practical reason or is is some legacy thing from older controls.

I'm sure there's a good reason I just can't think of one.
(So I'm coming from Heidenhain where the tool call contains all the info and tool lengths aren't cancelled (well I suppose they are temporarily)
by moving in machine coords etc)

In case you want slightly different offsets for the same tool.

ex:

Maybe doo to tool pressure, you may want a slightly smaller D on a longer cut surface than on a shorter wall surface?

Not sumpthing that comes up all that often, but .....

--------------------

Think Snow Eh!
Ox

Evenglischatiest · Aug 1, 2021

I sometimes use different D's when I have to turn big and small tight diameters with the same tool. If you need a 16" diameter on the back, and a 1/4" on the front, a slight offset in Y can easily cost you a few tenths. Separate D's let you tune them both in, without shimming up the tool.

On mills, I have engineers who like giving one sided tolerances. Sometimes I'll miss it when I'm programming. At the machine, it's easier to add a new D, than to fingercam a bigger/smaller tool path for that one sloppy callout.

mhajicek · Aug 1, 2021

Ox said:
In case you want slightly different offsets for the same tool.

Exactly. I've run several jobs lately in which a given tool will have two or three different D offsets for dialing in different features.

Vancbiker · Aug 1, 2021

barbter said:
Another way to adjust the tool (keeping the same offset number) for tight features, that i've just come across and used this week, is by using the attached.

That method can be ok, but without some care in programming can result in trouble should the program be aborted mid operation. Using alternate D addresses has fewer pitfalls.

Vancbiker · Aug 1, 2021

barbter said:
The variable I used was the H wear. The part had a tight limit floor depth (+/- 10 microns = 0.0004") and a following shallow angle scanned feature.
So after the floor and the Z retract, before the start of the scanned feature, I stored the existing H wear offset with a (#150) variable,
then had the following line with #10004 = 0 (ADJUST Z HEIGHT FOR CHAMFER).
This tool being T4 (a bull nose - hence me wanting the ability to adjust the Z incase the rad grinding isn't cock-on).
Then at the end of the feature (T4 toolpaths) on the last line before toolchange, I had this
#10004 = #150 ( DO NOT CHANGE. THIS LINE POPULATES WEAR TABLE WITH INITIAL SET VALUE FOR THIS TOOL )

So at the end of the tool, the existing tool wear value is automatically re-entered into the tool table. So next part, the previous H value (whatever that is) is back as was.

^ this is what I meant about careful programming.

Vancbiker · Aug 1, 2021

You need to set the appropriate wear value at the beginning of each op.

DouglasJRizzo · Aug 3, 2021

To cancel a G43 height offset, you would need a G49.
Depending on how the machine's parameters are set, BE CAREFUL, I've seen machines "take off" when the offset is cancelled.

Usually, when I'm done with a tool and send the spindle home with a G28G91Z0;, my startup line after the M06 looks something like this:
N20 G0 G40 G49 G54 G80 G90 etc

Now I know that all old offsets and comp are cancelled, cycles are cancelled, etc.

Search

Largest Manufacturing Technology Community on the Web

Search

G0G91G28Z0. cancelling G43 offset

markgerke

Plastic

Ox

Diamond

13engines

Stainless

angelw

Diamond

Booze Daily

Titanium

angelw

Diamond

srp61

Aluminum

Ox

Diamond

Evenglischatiest

Cast Iron

mhajicek

Diamond

Vancbiker

Diamond

Vancbiker

Diamond

Vancbiker

Diamond

DouglasJRizzo

Titanium

Similar threads