Making the Cut- Mastercam Toolpath Deep Dives

[Chally72]

Here's a fun multiaxis video that puts a toe in the deeper end of the pool and gives some insight into when to go after parameters like Max Angle Increment, Cut Tolerance, and Maximum Distance, as well as using the oft-ignored and slightly opaque "Smoothing" subpage of Collision Control. 

 

 

 

There are a few Making the Cut videos on our Youtube page already and more to come in the future, where we focus on some of the theory behind a specific toolpath or process. Hopefully this is valuable for some!

 

[Metallic]

Hi Dylan,

 

That was an excellent breakdown of some more advanced concepts on 5-axis smoothing and generating a good toolpath. Really great information! Sometimes it is hard to get a clear understanding of these ideas from just the help documentation.

 

I actually bought a slug to make this part on my machine...I would like to know how to approach the roughing strategy for clearing each of those pockets. I am having trouble keeping the tool from wanting to go behind the part when the part is tilted 90deg during transition moves.

 

Looking forward to more in this series!

 

EDIT: adding a photo for more clarity on the roughing

[Metallic]

I think I kinda got myself back on the right track from watching your 3+2 roughing video....adding a blank stock model seems to have tightened things up quite a bit. I somehow had never thought of doing that until I watched you do it!

[Chally72]

There are a few different ways we could trim the motion here and keeping the tool from reaching around the backside. (Even while using starting stock, etc, we still want to use one of these methods!) The first is to add the fixturing in as avoidance geometry. In the picture below, that would be the vise/etc. There are a few downsides to this, however-

-The stock must be perfectly positioned on the vise or you risk collisions OR have to unnecessarily puff the avoidance distances.

-Fixture modeling like this is really nice to look at visually, but extremely expensive computationally- especially if we're adding stock to leave and each individual surface must be offset before toolpath calculation can begin.

 

Another way to do this is to make a simplified solid that gets you avoidance around the fixturing without the complexity of 3000 fixture surfaces as your selection. Below, this cone was a nice way to keep the tool away from bad areas without spending a lot of time on avoidance:

 

Since Optirough with rest stock needs to have a containment boundary no matter what, though, the method I most often use for this kind of single-setup 3+2 work is to just draw a big semicircle like below and set it as my containment, where the wireframe line represents my hard boundary that I don't want the tool to go behind. This gives the path plenty of air region around the part and stock only in the direction I want it to- the table+ direction- and eliminates any wasteful/inefficient cuts where it would try to dive around the underside of the part by the vise to nibble away at edges, where I'm likely going to clean up the material anyway in the flip op for Setup 2. Around a part like this, you might see that semicircle Transform-copied 6 times to give me boundaries for my 6 pockets and my 6 Optirests. 

 

If you'd like to go over any more specific examples as you work through a roughing strategy, feel free to post the part or send it over and we can talk through options.

 

For those that don't know, there's another Making the Cut video that goes over 3+2 rest roughing on a similar part, utilizing stock models and a few other key tricks to make sure we're as efficient as possible. It doesn't go much into Metallic's specific question, since on that part there are clear interior pockets where we can simply use a Silhouette boundary, and don't run into the quandary of open air pocket ends and how to manage where the tool should or should not be at around the perimeter of the part.

 

[JrScott]

Hey Chally72,

I watched both of the videos and they were really helpful especially the 5 axis finishing where you added the points. I did have a question about the roughing video. You said in the video you set stock to leave at .02 on the walls and floors of your optirough path. What do you typically set your arc filter tolerance to, and do you use the smoothing settings?

thanks 

[Chally72]

Hey JrScott,

 

I actually don't often go after arc filter tolerances very much for the machines I work with. For arc filter and smoothing adjustments, the goal would be very similar to what we went after in the 5 axis path- What do we need to do to tailor the motion so that our specific machine likes it? The biggest thing that I see people do is to leave the roughing tolerance at the default 0.001" even when leaving, say, 0.020" stock. Take advantage of a bit of the stock band there to loosen up the roughing path- and same with applying the arc filtering. 

 

The end goal would be roughing (or finishing) motion that the machine can keep up with, so there are no slowdowns either because of code density choking the control, or acceleration rates that the axes can't handle. Speed changes = uneven chip load = tools die sooner. In that respect too, some controls (fanuc) really like the fixed segment length field here to evenly space the points. Find a settings combo that your machine is happy with, and apply that moving forward. Even if you can't visually pick out major changes, the final cycle time on a 5 minute roughing program is going to be revealing as to what your machine thinks of your tweaked points.

 

 

[motor-vater]

Honestly All the videos you guys have been making are the best thing mastercam has done for the end user well ever! Thanks for taking the time and keep up the good work. They should link these videos in the help manager So when you click help looking for a deeper understanding of filters and tolerances, these videos are there...

[Colin Gilchrist]

31 minutes ago, motor-vater said:

Honestly All the videos you guys have been making are the best thing mastercam has done for the end user well ever! Thanks for taking the time and keep up the good work. They should link these videos in the help manager So when you click help looking for a deeper understanding of filters and tolerances, these videos are there...

That is a fantastic suggestion! It would take some organization and maintenance on CNC Software's part, but the benefits would be enormous.

[Chally72]

Moving the help to a web-based format is allowing us to greatly expand upon what we offer for content. I believe that video and animation is one of the end goals of future help. We definitely want to leverage these Signature Parts series videos as help content anywhere we can, as I'm a hands-on learner and I think having help show you not just the functionality, but the real-world application, of a feature is critical to getting the most out of it.

 Have you checked out the help page on some newer features? The team has done a fantastic job of explaining some of these things with graphics and step-by-steps. Check out the linking help on 3D HST paths, for example. I didn't even know what the Maximum Lift field was for until reading down through the help. Paste that link in your browser to open it up locally if you've got the default install location:

file:///C:/Program%20Files/Mastercam%202022/Mastercam/help/en/Content/Toolpaths/Common/Linking_Parameters_3D.htm?cshid=11925