Adaptive Milling in NX CAM

Hello guys in this lesson i'll be using NX version 1880. I’m more interested today in the applications for trochoidal that were available in planar mill and showing users how they can duplicate that same type of functionality using adaptive machining. Let’s get started. Adaptive machining is in the mill contour area if you’re using that out-of-the-box set up for your templates

Here’s a dialog box for adaptive knowing so that we can learn more about the process. I’m going to give the operation minimal inputs.

Let’s generate then we see what result we get with the default values.

Obviously it’s cutting around the outside it’s not what we wanted. We want it to focus on the inside and we see that it’s cutting way too far down. Third problem is it looks like we’re cutting too deep with each pass we wanted. So let’s first fix that cut level that seems to be the easiest thing for us to straighten out and here on our range definition. I’ll select this face that’s as deep as we want to go.

Next let’s change our maximum distance to 80

Next, we need to set the boundaries beyond which our tool will not go. I’m going to create a sketch like a rectangle.

So we need to return to the adaptive milling operation and then assign that sketch as a trim boundary. Do need to be careful here? i want to trim the outside not the inside.

Let’s generate it

We see that the sketch the trim boundary is successful and preventing the tool from creating the peripheral geometry. We see a problem where a helical engages coming right down in the middle of the part it’s going to be very inefficient for this job.

Let’s depart from the operation and i want to go back and edit the sketch. I just need to stretch this rectangle out the exact size is not important. I just want to make sure i have room for that tool to sit down out here off the side.

I just need to regenerate.

Okay that’s looking much better. I am having my engages come down off the side of the part and there is no helical motion.I mentioned that there’s no finish pass here in this operation type.What this means then is that i’ll go into cutting parameters and i’ve got to add some stock make sure the stock is there in fact. I’ve already had that set it’s at 0.01.

Let’s verify 3D

So next i just need to create a finish pass so that i’ve got a similar function. I’ll choose to do this finish pass with the floor and wall IPW command.

We see our IPW shown transparently against our part geometry

I’ll select this bottom fase as our cut area floor and as i do so immediately.

Then we see a preview which looks good on the inside but i see little triangles where it’s going to try and cut these chamfers.

Let’s solve that problem. Now i’ll go into cutting parameters containment and here instead of extending the floor to the blank outline. we’ll just extend to the part outline and those are removed pretty much immediately.

Again we are going to work in the mode where we are just kind of sort of fixing.

It’s easier to see the effects of the different parameters. let’s generate again looking at our result and we are shaking out the tool it’s warning us about our flute length which is 0.375.

So let’s change the depth of cut to 0.3.

Regenerate it again. We get a better result and we do not we get the same result with a different error message and what it’s telling us. Is there’s so little stock on the side? That the tool overhang as it’s currently set isn’t going to allow anything to be machined..

We’ll go back to cutting parameters again and in containment then we would like to change our tool overhang here from 50% out to a 100%

So we intead of just bending around that corner let’s roll around that corner. So let’s just choose roll around and click okay.

One more generate that looks like what we are after therefore our finished pass.

Let’s create our second adaptive machining operation. Now we’ll be coming from the other direction and we’ll be using a smaller tool.

I’m going to need to straighten out the tool access this time

I have a sketch already created. So i’m going to turn that on. Use again for our trim boundary. Of course changing the side trim to outside.

Generate it.

Well that certainly is machining the area we wanted to but it’s also rhema sheen in the inside which has already gone. At this point to understand what went wrong here we need to go back and look at containment clearly.

We can see that by default this command is not using the in process workpiece. So we need to choose use 3D.

So we are hoping to solve two problems we would like to machine only back into these roots and we want to get rid of this helical engaged.

Let’s generate it.

That looks successful it’s using 95% of our flute lenghs that’s causing it to make three passes on the way down. Our engages are not helical and they’re off in the open space our trim boundary.Let’s look at one further alteration we migh make to our program. It’s common to use reground cutters for hard materials and we might want to turn cutter comp on. So that the operator out the machine could quickly change the diameter of the cut.

We will go to our start of path and i’m going to look for the cutter compensation. Then my mode is to turn that on and i’ll take the defaults here of on before each engage and off before you to retract.

That’s really all that’s required when post-process this now with that start of path event i will get G41 and G40 as part of that tool path. Thank you for reading see you next time.