Incremental vs absolute in Mastercam 2020

When working with most 2D milling toolpath on Mastercam 2020 (Contour, drilling, dynamic mill, etc.) the last thing to be set when creating a toolpath is the depth of the operation in the Linking Parameters tab. This rather easy parameter can get quite confusing when it comes to the options of Absolute, Incremental and Associative.

But what are these options, what do they do to my toolpath and how could I use them to not only improve the effectiveness of my toolpaths but reduce the time I spend programming?

To explain these let us look at a drilling operation. Let say we have a block 100 x 80 x 50 that we want to drill 3 x 10mm holes into.

Now let say that these 3 holes are at different depths. In this example, I made the depth of the first hole 10mm, the second 25mm, and the last 40mm.

For this to work, we must place points entity in the bottom of each hole, as can be seen in red down below. When we start the drilling toolpath, these are the points that we would like to select.

Once we have selected a preferred tool and parameters let set the depth to -40 mm absolute.

The results of this can be seen below.

What is happening here is that when you select absolute, the depth is taken from the origin of the part. Because the origin of the part is at the top of the part this means the depth is -40 mm from the top. This also means that if the origin was set to the bottom of the part, we would then have to change our depth to 10mm to get the same result (With the block being 50mm and we want to drill 40mm deep).

Now, let’s go back into the parameters and change the depth to -40 mm incremental. If we regenerate our toolpath, we will get the following result:

You can see that what happened now is that the depth is no longer taken from the origin at the top of the part, but rather from the point that we have selected. What this means is that if we would then change the depth to 0 incremental the drill would go to the depth that we want in each hole, as seen below.

This will not only save you time, by not having to create a drilling operation for each hole but will also shorten the length of your NC code as well as saving time on programming, leaving you to decide what you are going to do with all that time saved.

This, however, doesn’t only work for drilling but can be used for most of the 2D milling toolpath. For example, take a rough operation down below.

Here we have three pockets of 100mm x 50mm with depths of 25mm, 40mm, and 50mm. We will use a 10mm flat endmill with a 10mm stepdown and a 10% stepover.

This allows us to chance 3 toolpaths into just one, keeping all our parameters together.

I would advise you to play around with these options for your Depths, Top of stock, Retracts and Clearance and see how this simple change can influence the effective and time spend programming in Mastercam 2020.