Tool Offset Compensation

[jsanchez177]

I created a program that used a contour milling cycle in finishing a pocket. A 3/16" 4 flute End Mill was used for generating the code. The technician that runs our VMC (an experienced manual machinist but somewhat new to CNC) had came in and asked me if I used a tool radius offset compensation on the contour in which i said yes. After running the code he stormed in all fired up telling me that the size of the pocket was off by the radius of the cutter. In inspection I noticed that he had entered in the radius of the cutter as the offset for the contour milling block. Therefore I told him that if he specified a zero offset the part should machine to spec. He got all excited and told me that, that defeats the purpose of using a Tool Radius offset if he can't just enter in the radius of the cutter that he is using. Anyway, make a long story short this technician has a history of having a "hot head" which makes him difficult to work with. Can anyone help explain to me what most likely happened in my situation and if i should change my post to how he wants it (where he enters an offset for all contour features which equals the radius of the cutter he is using)? Or if I should continue creating the post with a cutter in mind in which he then could calculate an offset if he wanted to use a different radius cutter?

Phew, I hope that made sense. Kind of frustrating, he's a my way or the highway kind of guy and needs to cause a scene to get a point across.

Thank you so much in advance. I truly appreciate knowledgeable people that share their wealth on forums like this.

[broby]

O wow are you wrong and the "Hot Head" correct!
The whole point of programming a profile using cutter radius compensation is so that you can set the exact radius of the tool at the machine.
This way, if your cutter is reground, you can still use it with the program without having to reprogram the job.
When you program, you should be outputting true geometry, i.e. sizes that you can find on a drawing, not a compensated profile.
If you program an offset profile, your operators will be having a hard time translating where the tool is supposed to go to when looking at the drawing.
Good luck dealing with the "Hot Head" but this time around he is correct in what he did and said.
Regards
Brian.

[mfgbydesign]

Brian I'm sorry to disagree with you.
There are two methods for using "cutter compensation" (radius or diameter based on parameter settings in the control). Lathes are a different story and I would agree with you had this been a lathe issue. Here they are:

1. Manually programming using print dimensions, enter full radius (or diameter depending...) and let the machine control calulate the cutter centerline.

2. Use a CAD/CAM system to calculate the cutter centerline coordinates based on designated tool size determined by the programmer, and enter the DIFFERENCE into cutter compensation (also refered to as wear comp. in this case).

Option 2 is the prefered method, as it: a) minimizes control "add-on" blocks which can produce unexpected machine moves and requires excess lead-in values; b) allows for one-time off-line calculations to be performed and can save processing time at the machine control; c) enables accurate simulation of the machining process and toolpath verification which is an often overlooked advantage of the current state in CAD/CAM software; d) there are many cases where the programmer may not want to use CDC or can't because of complex surfacing in 3D with ball or bull cutters.

HTH, Steve.

[jsanchez177]

Thanks for the replies and thank you 'mfg' for the explanation. This is how I understood it but just needed to be reassured. There was a time when using dimensions from the drawing and offsetting the path by the radius of the cutter was an effective way of checking your program matches the spec drawing. Now with the advancement of CAM software and simulations the alternative method seems to be much more useful. Not that either are incorrect. Thanks again! :-)

[mfgbydesign]

"checking your program matches the spec drawing"

The software I use lets you compare your completed verification model against an stl file from the CAD model, displaying deviations by color for the ammount + or -. If you program a part with hundreds or thousands of features this is extremely useful. It seems I always miss something or gouge the part. Now I can identify these errors and make corrections before I run a piece.

[G0G90]

Diplomacy is the key "opportunity" here.
I agree with both methods in their respective controls.
Sometimes, working with a "hardened / experienced" technician, creates a differential in approaches to manufacturing.

Simple solution; inquire the tech on the process. Explain how using a zero-comp can be to his benefit by allowing "control" with absolute radial adjustments on his cutter.

The innocent act of user-input, can be enough to ease tensions.

Oh, and ALWAYS document which method is being used in the header.

[jsanchez177]

This is very good advice I appreciate it.

[broby]

G0G90 has stated exactly what I would expect from programmers working here.
You can NOT blame the operator for setting up the machine one way (the correct way in my mind, and that is MY opinion!) and getting a part wrong if YOU (the programmer) have not informed the operator as to how you have programmed the job.
We ALWAYS include a full description of what has been included in the program, what tools are used, any notes on how the tool is to be setup, and what fixturing is used.
Zero Set information is also included in the titleblock of the program.
Because we are basically a semi-automated 'jobbing' type of workshop, jobs are changing over very quickly, lots of repeat orders, but if the programmers fail to let the operators know exactly what and how things are programmed you can be assured the brown stuff is going to come flying your way real quick.
I agree that Cutter Radius Compensation can not be used for every operation. but hey, If I am doing a 2.5D profile, it would be a rare program that does not use G41/G42 as required.
If you setup your start-end points for the profile, you do not end up with large startup/end comp moves anyway.
We use an extensive range of Solid Carbide Endmills from Sandvik that cost a fortune and are constantly being reground, if I were not to use Cutter Radius Compensation I would be reworking the program all the time. No thanks to that idea!
It also, obviously, depends on how your target machine is to be programmed and used. You need to establish standards between the programmers and the operators as to how different operations are to be done, and stick to them!
This way everyone knows what to expect. Do you want to be fixing up something at 2:30am? Not me!
Since you posted this in the Camworks forum you must be using Camworks?
How do you find this software?
Is your post giving you accurate output as expected?
I have found that you have to be careful to not "double" up on your compensation when doing profiles, as you can select a set of conditions that allow Camworks to output a tool path that is offset by the radius of the cutter and with the Machine Compensation activated also. Thus if the operator puts in 10mm cutter radius for a 20mm diameter tool and Camworks also offsets the profile by 10mm, you will be a long way out.
What do you do if you have programmed a profile using a 20mm diameter tool and then there are none available (and the supply is due the next day) but the customer is demanding delivery today?
If you program using true geometry and allow the machine to "compensate" by way of G41/G42 then you would be easily able to substitute any other suitable cutter and get your job done anyway.

My 2cents worth.
Cheers
Brian

[davy182]

Our shop has come across some of the same issues, with having multiple operators/cad drawers. We have had fun redrawing things because dxf where drawn for a specific bit and whoops we broke that bit. I have tried to simplify things by saving things to spec in vcarve with the cutting profiles. All we have to do is change the profile and output a new tap file.

And the part I love the best about it is there is no reason to keep the tap files if it is stored in vcarve. This way no more guessing was that tap the good one. Just open up the vcarve file, and if everyone did their job right notes should pop up upon opening for the operator to read, then make any profile adjustments and save your tap file and off you go.