MC Finish

In a nutshell  
How it works  
In your shop
White paper  
Purchase info  



Products : MetaCut Finish : In Your Shop


MetaCut Finish & Pro

In Your Shop

What should you expect from MetaCut Finish?

To answer this question each of the following points will be addressed:

  • Accuracy

  • Reduction of machining time

  • Finish quality

  • Polishing time

  • Machine maintenance


"I would recommend this software to anybody.

I barely have to touch my electrodes after machining when using it."

Jack Strohecker
(Vice President)
Accu-Mold & Tool Co. Inc., PA, USA
Used for: Electrodes



Accuracy- The accuracy after using MetaCut will be exactly what you specify. However it is important to realize that accuracy starts back in the design stages. Relative to the machining process, when we speak of accuracy, we usually mean how accurate relative to the original CAD model. This is easy to calculate.

If we assume that the CAD model is perfect. (it's not). Then there are two more places for error to be produced before you begin the actual machining process. The first place for error to be produced is in your CAM system. You specify the amount of error when you make a toolpath. This is usually called the "Chordal Deviation" or "tolerance" of the toolpath. If you keep in mind that virtually all CAM systems produce toolpaths that represent the curved surfaces of a part as short straight lines, it is easy to see that here is where the error begins. The idea is that you produce a path with an "acceptable" error. It would be fair to say that everything you do to produce a mold has an acceptable error built into it. There is no such thing as perfect, only close enough. Your job as a machinist is to make the final part "close enough".

The second place for error to accumulate is in MetaCut. MetaCut must fit the point to point data with arcs or curves. You specify a tolerance and MetaCut produces the new entities within the tolerance you specify. You must keep in mind that the error in MetaCut is added to the previous error in your CAM system to produce the final total error relative to the CAD model. If the total acceptable error for your part is .0005", you need to add the error in the original toolpath to the error in MetaCut and make sure that the total is under .0005".

This brings up an interesting point. Different CAM systems specify the tolerance in different ways. There are three primary possibilities as follows:

1) The tolerance is specified as a single number but is actually a plus or minus tolerance. In this case if you specified a tolerance of .0003 your toolpath could go below the original surface by .0003 and above the original surface by .0003 for a total error of .0003 + .0003 = .0006".

2) The second method is for the CAM system to specify one number that represents the total error. In this case a tolerance of .0003 would allow the toolpath to go below the surface by .00015 and above the surface by .00015 for a total of .0003". As you can see, with the same apparent tolerance, this method is actually twice as accurate as method number one.

3) The third way to specify tolerance in a CAM system is to allow the user to specify two (2) tolerances. One tolerance represents the deviation into the surface and the second tolerance represents the deviation out of the surface. This is often called "in tol" and "out tol". In this case the user might specify .0002 in tol and .0004 out tol for a total of .0006" deviation from the original surfaces.

As you can see from the above samples it is important to know which method your CAM system uses. If you don't know, you do not know just how accurate you are making your part. MetaCut uses method number one (1). You specify one number for the tolerance and MetaCut allows the new entities to deviate from the original point to point information both inside and outside of the original points.

If you are unsure of the method your CAM system uses, you can probably find out just by running MetaCut on one of your files. Because your CAM system data already includes the error you specified, it is nearly impossible for MetaCut to fit new entities to a tolerance smaller than you specified in your CAM system. You can take advantage of this fact to find out what your CAM system does by running the same file many times in MetaCut using smaller and smaller tolerances. When MetaCut can no longer fit arcs to the point to point data, you are probably very close to the tolerance which was specified in the original file. Because you know how MetaCut's tolerance works and you know that MetaCut can rarely fit data with more precision than the file it was given. You can calculate the method used by the original CAM system. Following this paragraph are two examples.

Example 1- You make a file in your CAM system which uses a tolerance of .0001". You import the file into MetaCut and try to run the file at .0001", you find that it does not fit arcs in the places you expected it to. You open the tolerance in MetaCut up to .0002 and you find that it fits arcs very well. In this case the CAM system probably uses method number 1 above. In this case the most appropriate tolerance to use in MetaCut is just slightly large than the original tolerance specified in your CAM system.

Example 2- You make a file in your CAM system which uses a tolerance of .0001". You import the file into MetaCut and run the file with a tolerance of .0001", you find it fits arcs in all the places you expect it to. Then you run MetaCut at .00005" inches and find it seems to be missing some places where you expected it to fit arcs. Then you try .00006" and all the arcs are back. Your CAM system probably specifies the tolerance just like method number 2 above. The tolerance specified in the CAM system is the total deviation from the original CAD data. In this case, the most appropriate tolerance to run in MetaCut is just over half the originally specified tolerance.

You should notice from the above examples that the tolerance you run in MetaCut is usually directly proportional to the tolerance you ran in your CAM system. The final tolerance in MetaCut is usually one place of precision greater than the original tolerance in the CAM system, once you allow for the difference in the method of specifying the tolerance.

Reduction of machining time - You should see a significant reduction in machining time. The actual decrease in machining time will vary from part to part and from machine to machine, but reductions in machining time are typically 15 to 50% percent with high speed controls and often 200-400% with conventional controls, best of all, because of the feed control and mode switching in MetaCut, you will see this reduction in time without adding error to the machining process. Depending on your current methods you may actually get a more accurate part even though you are able to make the part in less time.

Finish Quality- Due to the additional feedrate and mode controls available within MetaCut you should see the surface finish of your complex shapes get better. Of course, a better surface finish means less hand polishing, another time intensive part of mold manufacturing. Less hand polishing means a more accurate part.

The actual increase in surface quality depends on many factors which include the following list:

  • The construction of your machine tool and the control on your machine tool. If your machine is an old machine with an old control you should see very large differences in the quality of your surface finish. If your machine is a modern high-speed machining center the improvement in surface quality will be less obvious. (you will still be able to machine the part in much less time)

  • How well you collected data for your feed control table.

  • Whether or not you used the exact stop/continuous mode switch.

  • What tolerance you specified in the CAM system and in MetaCut. If the total tolerance of your CAM system and MetaCut is significantly larger than the tolerance you usually use with your CAM system alone, your surface finish will suffer.

Polishing Time- Just as in finish quality, there are a number of factors which determine the amount of finishing time you will need on your parts. If your parts do not require a 'mirror" finish you may be able to eliminate almost all of your polishing. The actual reduction in polishing times will depend on how well you set up, understand, and use MetaCut. The better you understand the factors which go into producing an accurate part, the less polishing time will be required. Remember, surface finish and reduced polishing start with accuracy.

Machine Maintenance- This is almost impossible to quantify but there is a physical difference in the "feel" of the milling machine when it is running toolpaths optimized by MetaCut. Even on a high-speed machining center there is a quality of smooth running which can be felt just by touching the machine while it is running. Also on your machines which do not have high speed machining capabilities, the mode switching of MetaCut will prevent a hard "bump" as the machine reaches the end of one cut and suddenly needs to travel in exactly the opposite direction. The very nature of a toolpath which has been optimized with MetaCut is to produce a smoother operation. This is why even a high speed machining center can achieve a significant decrease in machining time. The smoother path, allows the machine to maintain a higher average feedrate, without inducing additional error.