Surface Finishing Strategies - 3D Contour - Smoothing, Tool Offsets, Etc
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
I do not have much experience in mold work, but have worked in stamping most of my life and have done some pretty complex form tools. Most of this experience, albeit limited, was on higher end machinery, like a Hermle 5ax.
Lately I have been working on some tooling for a customer, which has really given me a run for my money attempting to use Fusion. There isn't a flat or parallel side on the part (except the end), and often times it is a frustrating and time consuming guess and check process to determine what works.
This is not meant to be a comprehensive post by any means, but I just want to share a few things that I have found worked pretty well.
If you have any questions about Smoothing, this is an excellent basis to begin:
https://forums.autodesk.com/t5/fusion-360-computer-aided/understanding-smoothing/td-p/6636189
The part I am working on is a cylinder of sorts, with lots of faces, protrusions, and goofy stuff the customer dreamed up. The model would be excellent to share, because this would all be much more informational, but due to ITAR, customer requirements, and lots of other political BS, it is best left out. And honestly, tying it specifically to a model tends to change people's understanding. The few simple tips I am going to post really apply to any 3D machining.
First, Ball endmills. I see a LOT of people posting using 3D ball endmills for 3D form work. Ball endmills really are not meant to be used perpendicular to the work piece. They are common for form work, but typically in a multi axis machine. The majority of ball endmills are not center cutting, and as at center they are "not" turning, they cut poorly. Ball endmills are best utilized with a 10-20 degree angle (I usually shoot for 15). Easy to do in a 5 axis, not easy to do in a 3 axis. If your part has sloped walls, perfect! Often with 3D forms however, you will transition through many faces, and that is when issues crop up.
Bull endmills, however, are great for form work as the tool is cutting on the outside edge. Typically you can get away (sometimes!) with a bigger diameter tool, providing a more rigid cutter.
Here is what I wound up doing with my recent piece of tooling. Keep in mind, I do not have a full 4th axis, but rotate my work on a dividing head. Works the same, I program in sections, and rotate as necessary. Been doing it this way for years and started out machining manually with dividing heads. So far it has been humorous, at times, it is faster to machine a complex form manually, rather than bicker with Fusion to try and convince it to make what it views as a strange cut. (I don't think Fusion was made by those w/ "old" machining knowledge)
So here is what I found best to work out the tool. I tried many of the other 3D strategies but none seemed to efficiently work. Most of the time, they wanted to cut the part in half.
3D adaptive clearing to rough in the shape leaving .020 stock both radially and axially.
3D Contour to semi finish with a 12mm 6FL 1mm CR .005" stepdown .005 stock both radially and axially.
3D Contour to semi finish with a 12mm 6FL 1mm CR .003" stepdown .002 stock both radially and axially.
3D Contour to finish with a 6mm 6FL .5mm CR .001" stepdown stock both radially and axially.
Normally I would have prefered to finish with a fresh 12mm with 1mm CR, however due to the geometry of the tool 6mm was the largest I could use and still correctly generate some of the features.
To tie into the smoothing aspect, I ran into several issues, one a recurring one I have had with Fusion, and several new ones. The previous thread mentioned above does a great job outlining the variances in smoothing and how to shoot for a target. However, it does not provide much info for higher precision "goals". For example, on my finish pass I ran .0001 tolerance and .0004 smoothing. Which was necessary to get the finish I needed to clean up the part with minimal hand work. This was also necessary DIMENSIONALLY, as I have found the majority of the dimensional error is created out of the programming. Much of this depends on your post and your machine. Sometimes it takes a LOT of tweaking and experimentation to get dialed in.
The high tolerance also presents another problem on the machine side that you need to be cognizant of. Two fold issue really, the size of the program and the number of lines of code. They go hand in hand but they are two separate issues. If I want to mill a PRECISE 1" square, it is necessary to set both the tolerance and smoothing to an exceptionally SMALL setting, which produces an ENORMOUS amount of code, for four linear movements. This is doubly important if you want high surface finishes. My machine will for some reason, error out at 100,000 lines of code. I am working with the machine tool manufacturer to change this, but for this part, it required me to break the programs into 15 degree segments, and then work all 8 segments to blend in correctly. This is frustrating, especially with the particular segment is a linear 1" cut, swept into a radius, and about 3/4" length of cut. Fusion produces 8 lines of code to output one pass, which to me, should be 3 lines. Part of this is due to Fusion wanting a radius move at each linear segment, which you cannot seem to turn off in 3D contour. An issue in this case, because I want crisp sharp corners.
One last issue to consider when you are doing 3D surfacing. On one segment the tool nicked a corner for some reason that I could not track down, and it required re-running all 8 segments. This, to me, is frustrating, as there is no cutter comp for 3D Contour and you must manually input -.0005" into stock to leave, then repost, reload, and rerun.
Certainly don't take this as a be all end all. I have been using fusion for a little over a year. It has to be the most frustrating and irritating modeling and CAM system I have used in my career, so my hope with this post, is to pass some of that hard won knowledge onto others.
