[jdgromi]

Hello!

How can I use the offset wear to correct the axes X and Z when my diameter is greater or smaller that the value of my program?

Best regards

Jean-Denis

[stevo1]

What kind of control are you using? If you have a wear offset page then which ever tool offset you are using ex. H5 then under the wear for 5 X or Z put the value of how much you want to change + or -. Depending on how you tools are offset usually you can put -.005 in the X wear and if your tool geometry is X5.61 then your tool will run as 5.605.

I usually don't use wear becasue most of the time people don't bother to check that when changing inserts. If it is a high volume job that requires the wear to be used and everyone knows this then you should be fine. I typically use this when dialing in a part or tool and once I have achieved this then I dump my wear number into the geometry number and clear the wear to 0.

Stevo

[jdgromi]

Hello!

My control is a Fanuc 21i. I have made the geometry offset correctly for the tool 10 but whent I run the program, the diameters are 0,004" below. I want to correct this error but I don't know where.
My tool is hight speed steel and my part is in PVC. I run the lathe in slow speed like 400 rpm.

Best regards

Jean-Denis

[sinha_nsit]

Specify -0.004" as wear offset, though I am not 100% sure whether the sign should be positive or negative, as I have never tried it. Please try and let me know.

I normally do it in an indirect manner:
If you are getting a lower dia, say 9.95 mm instead of 10 mm, it means that when the tool is programmed to be at X10, it is actually X9.95 position. This means that X10.05 would actually be X10.00 position. So, bring the tool manually, in JOG or HANDLE mode, to X10.05, and repeat the offset setting process to make it 10.00. And, this need not be done at 10.05 only. You can also make, say, X100.05, the X100 position.

[stevo1]

Jean,
You have a few options. If you are always running .004" below diameter you could change the geometry of the tool to match. That's only if it is always running below. If it is only because of the tool or the part/material you don't want to do so as then when you put a different job on it will not run to the correct diameter (well at least it would run big).

IIRC the way to look at wear adjustments is if it is a + geometry then if you go +.004 with your wear then the machine takes the 2 numbers (wear+geometery) and now it thinks your tool is longer in turn staying further away from the part. If you were to put -.004 it will think the tool is shorter and come closer to the part.

Ok I went and reread your post. What do you mean you don't know where to make the adjustment...you can't find the wear screen? If you press your offset/settings hard key until you get to your offset page were you enter your geometery then the options of the softkeys should be WEAR, GEOM, WORK..., OPRT. If you press the WEAR it will take you to the table that looks just like your geometery page except they should all be 000. That is were you make your adjustment. Now if you do the same as above except your options on the softkeys is OFFSET, SETING, WORK,..., OPRT then you do not have the option activated on your control.

Stevo

[sinha_nsit]

... If it is only because of the tool or the part/material you don't want to do so as then when you put a different job on it will not run to the correct diameter (well at least it would run big).

Stevo

He has to change the geometry offset value, because the offset setting is not correct. Once it becomes alright, further adjustment should be done preferably by wear offset, to take care of tool wear after some time. Finally, when the tool insert is replaced, wear offset should be made 0, and the same geometry offset will work.

For offset correction, if you choose the method I suggested, you have to type 10.00 (after bringing the tool to X10.05, as displayed on the screen), and then press the MEASUR soft key.

If you cannot use geometry or wear offset due to any reason, you can work with only one tool. And you have to modify work offset for offset correction, in such a case.

[stevo1]

He has to change the geometry offset value, because the offset setting is not correct. Once it becomes alright, further adjustment should be done preferably by wear offset, to take care of tool wear after some time.

I have made the geometry offset correctly for the tool 10 but whent I run the program, the diameters are 0,004" below.

I assumed that his tool geometry was correct based on him stating that he did it correct and when he runs the part it comes out small by .004”. Yes I would believe that this is a geometry problem and he is just a bit off when actually doing the tool offset. But there can be many reasons that the part is running .004” small other then the geometry. I think what he has to do is figure out why when doing his offset or measure function is the tool geometry running .004 off.

LOL I think we are getting a little OT of what Jean was originally asking.

I think that if he is not seeing the “wear” softkey then he does not have this option installed and he will have to do as you and I are discussing and just stick the .004 in the geometry and call it a day.

Stevo

[sinha_nsit]

Everybody does offset setting "correctly". But, since it involves human judgment (whether or not the tool has touched a surface), chances of errors are always there. And if the procedure is repeated all over again, there is no guarantee that the offset setting would now be correct. In fact, if the person is not very careful, the error may even increase! So, the best way is to edit the geometry value. Of course, in case of automatic tool setting using a touch probe, this problem would not be there.

[sinha_nsit]

Specify -0.004" as wear offset, though I am not 100% sure whether the sign should be positive or negative, as I have never tried it. Please try and let me know.
.

Today I verified how wear offset works on the machine (rear type lathe). When I specified positive values for X and Z wear offsets, and executed T0707 in MDI mode, the tool moved in the positive directions (i.e., away from the workpiece) by the specified amounts, without changing the position display. This means that the obtained dimensions would be larger, for the same program. This is what Jean wants. So, he should specify +0.004" as X wear offset value, not -0.004" as suggested by me earlier.

This also means that if we are getting larger diameter because of tool wear, this can be corrected by specifying negative wear offset.

Stevo,
If you find that I am not correct, you should correct me immediately, without any hesitation.

[stevo1]

Sinha,
You are correct. That is what I stated before. I remember discussing this in another thread before. I will post it if I find it. The only thing to look for is the parameters set for radius or diameter. There are ways to change this even when programming in radius. I believe on this control it is done with parameters 5040.0 & 5004.1

When I set up VTL’s for production I had OD tool geometry as distance from tool tip to ram center. This was moving positive so the offset was positive. The ID tools were from tool tip to ram center but this was a negative direction so the geometry was negative. Now when you adjust wear it adds geometry + wear. It was very easy to look at the machine and say if you want to move closer to the part(negative direction) then adjust -.004 for your OD tools. ID tools the same just look at the direction of the machine. If you want to move closer to the part(positive direction) then adjust +.004 for ID tools.

The easiest way to remember is just do the math. Tool geometry is 7.534 wear adjustment -.004 your new tool length is 7.534+-.004=7.530. Shorter tool moves closer to the part, larger tools stay further away.

Stevo

[sinha_nsit]

Thanks for confirmation.

I had not realized that for internal tools the wear offset should be positive, because then only the tool will move towards the job.

[stevo1]

Sinha,
It does not have to be that way. You can set it up anyway that you want, This is all determined how you set your home position and your geometry relative to that. I just always found this the easiest way.

To help visualize this physically put your OD turning tool on the OD of your part. Now moving closer to the part is negative machine direction and further away is positive machine direction, and that is how you would adjust your wear or geometry +/- machine direction. Now physically put your ID boring tool on the ID of the part. Moving closer to the part is positive machine direction and moving further away is negative machine direction, and that is how you set your wear or geometry +/- machine direction.

There are many ways to skin this cat.

Stevo

[jdgromi]

Thank you everybody

Your help has been very appreciated.

Yesterday I fixed the geometry, I took a light cut and I wrote the mesure in offset geo X2,000 tool 10. After I ran in CNC mode, I took a other cut and I read 1.996" 0,004" below. Then I changed my wear offset with the number 2,004" . Now I read in the screen table wear offset X 0,004". After I took a other cut in CNC mode and I read the good value.

Best regards,

Jean-Denis

[stevo1]

You are welcome..

Stevo