Improving 3d surface finish - Improving Fusion Code

[M&GToolWorks]

I have done quite a bit of work using Fusion generating a 3d profile with a bull nose endmill, sometimes it comes out great, and sometimes... less than great. I have never been able to pin down specific settings to improve. 

Yesterday I started machining a part, that like many other parts, I am generating a 3d profile using a bull nose endmill. I have done several jobs like this in the past, with satisfactory results. This time however, the results are not satisfactory and I cannot understand, or see, why. It was humorous to me, because on the same part, fusion generated a 3d surface using the same endmill, that looks nearly ground. 

The frustrating part, had this been a one piece job, was the time spent trying different tool paths, all with varying degrees of success and failure. With the time spent on this, I could have set the job up on my 1942 Brown & Sharpe and had it cut with as good, or better, surface finish. The next 49 wouldn't have been quite as quick... 

I have attached a file with several attempts at tool paths to see varying effects. I would be interested to see what the community can come up with that may help me achieve an acceptable finish. I am sure (Seth, I'm looking at you) there is some obscure check box buried in a menu that will give me beautiful finishes on this surface. 

https://a360.co/2SlDRgU

[MoshiurRashid]

Try decreasing your stepover value.  This will improve 3d curve surface finish.

[M&GToolWorks]

My apologies, I should have taken the time to explain better. I am curious if you looked at the part file and tool paths? The cusps are not the issue. I ask because decreasing the step over seems to make the tool paths worse. Decreasing the tolerance under passes equally seems to make the tool paths worse. 

If you experiment, a .005" stepover appears to make a better surface than .0005" ignoring the cusps. Making the tolerance .001" instead of .0001" seems to improve the surface. This is counterintuitive to me... hoping someone can explain and help. 

The issue is not the cusps, the issue is with the code that Fusion generates. If you take a look at the tool paths included in the example file, and simulate them, you will see that quite a poor surface is generated. 

[MoshiurRashid]

Hi,

I saw your file and I've found some complexity here. I'm checking it out with some other ways. There can be a fact of tool selection, whatever I'm checking that and get back to you soon if I get the solution for it.

[johnswetz1982]

" If you take a look at the tool paths included in the example file, and simulate them, you will see that quite a poor surface is generated."

The simulated image is of fairly poor quality. You can zoom in to resize the mesh that is generated for the simulation but it is still a mesh. Does your actual workpiece show a poor surface or only the simulated one?

[M&GToolWorks]

I look forward to any input you can provide. 

[M&GToolWorks]

I only ran a couple tests as I did not have time to cut sample material and make some samples, however the poor surface finish that is simulated, does approximately match the poor surface finish of the part. 

If you select one of the operations and look at the tool paths, you can see where they are not an even face, some extend further in, they do not follow the curve. 

I have not machined each of the operations I created, however. 

[daniel_lyall]

What machine do you have and what control does it have.

Some of it is coming from the model it's self the surfaces of the area being cut is ugly run a surfaces inspection if you run the first 4 inspections you will see some areas fusion just does not like at all this is internal to fusion it is hard to get a clean surfaces at time, I have one 4th axis continues toolpath out of the 100's I have tried to get working, and it is the surfaces doing it.

I have managed to bugger up something I will post what I would do when I can get fusion working properly again.

[M&GToolWorks]

You'll have to explain surface inspection, is that something in Fusion? 

Machine is a Brother S1000 w/C00 control, amply capable of this type of work. 

I know from previous experimentation that the machine is capable of producing impeccable finish work. I have had Yamazen down for applications training and we ran some side by side comparisons of MasterCam and Fusion.... lets just say that Fusion really showed its price point in comparison. 

The code Fusion puts out has been a gripe of mine from day one... but what do I know, I'm just a dumb hillbilly machinist. 

[M&GToolWorks]

So ultimately this is just limitations from Fusion?

[daniel_lyall]

This is your model it is hard to get a good clean surfaces in fusion (I wish they would work on this more) you can get them.

With what needs cut it is just useing the correct toolpath and tool, if you change the tool to a ballnose there is a diffrences in all toolpaths you have tryed it is small but is there also a bit of a graphics error is going on as well.

Green is good red is bad

What I like to do is turn everything off in the toolpath bar the cutting moves, this way you can see quite quickly if the toolpath is going to be rubbish or not below is useing ramp with a ballnose.

This is the parallel tollpath with a bullnose you can see it is rubish.

With a ball nose it is better but still a bit rough comepeared to the ramp toolpath above.

I have the time to do all this playing around I know you wont.

Anyway my atempted is attached 

[HughesTooling]

Unfortunately Fusion doesn't give you any control over the mesh in the CAM workspace apart from surface deviation. Just using a tight tolerance doesn't work well for surfaces with subtle curvature as you end up with long thin triangles. You can work around this a bit if you convert the body into a mesh in the design workspace where you have more control. 

Screencast below shows how to create a base feature and convert to mesh. Not sure why you selected the finished body as the stock it makes it difficult to view in the simulation, I just changed it to a relative boc stock. You could also improve the toolpath if you extended the surface you want to machine so you machine past the edges. I've attached the file, only modified the one op.

Mark

[M&GToolWorks]

Thank you both for your replies. I set up my 1942 Brown & Sharpe and cut the appropriate leads. Took some time since it has been quite awhile since I have done that type of work. Even with .002" spindle run out, the finish was better than what Fusion generated. 

 I don't know why when I hit reply, I cannot include your quote to answer specifically? It used to be when I hit reply it automatically included the persons post that I was replying to? 

Daniel, 

Thank you for taking the time to show me that. It is funny, when you mentioned surface inspection, I spent some time googling to try and find out what you were referring to. I had no idea "curvature map analysis" existed, nor would I have thought to use it. Unfortunately I have to fall back on my "I'm just a dumb hillbilly". When I create a surface, I assumed that Fusion created a surface. That is the extent of my knowledge. In 5+ years of using Solidworks for all my CAD/CAM work, I never once ran into this issue. I guess this is the point where I learn and understand why Fusion costs what it does comparative to SolidWorks? 

I will save your suggestions for next time to try out. I prefer to run bull nose instead of ball cutters primarily for speed and surface finish. I can run bull nose at much higher feeds and speeds and typically they result in better finishes depending on the type of work. There is plenty of angle in this part, that a ball would work well, and I will try that on my next batch of parts. 

I appreciate you taking the time to show these ideas and help me understand better. Your right in that I do not have the time to play. As mentioned, I am pretty ignorant when it comes to things like fusion. Whether with past Autodesk products (primarily autocad), Solid works, mastercam, etc... I never spent any time that I remember with "workarounds" or tweaking part geometry trying to get them to a machinable state. Because of this, I now keep an excel spreadsheet that is my "solidworks" fund. Whenever I lose money on a job because of Fusion, I record that loss. I'm a machinist, not a computer scientist. I suppose it is my ignorance, but I shouldn't need to do a "curvature map analysis" or a "mesh conversion" to be able to machine the parts. This is all several steps backwards in the world of machining. Perhaps I should take a step back, am I doing something incorrect with my modeling? I see folks online machining far more complex, far more intricate items with Fusion, and none of this tweaking or working around is necessary. Perhaps someday this will make sense. Until then... I'll keep adding to my Solidworks fund. 

Mark, 

Thank you for taking the time to make this video for me. Is this a normal process for you with the models that you machine? This mesh issue, would this explain why I see part variance and issues with Fusion code vs Mastercam? 

To answer/address some of your other commentary: 

the sample part is a piece of the part that I made. Because the way Fusion handles stock, I have to model my stock, select the model body as stock, then simulate. That carried over to this sample when I stripped away the rest of it, sorry for the confusion. 

In the past, on almost every curved surface that I machined, I would extend the surfaces to allow for Fusion to (in my opinion) correctly machine the curved surfaces. Someone on this forum made me a great little video, such as the one you made for mesh conversion, and I wrote a little "process" sheet for myself on how to do that. At some point recently Fusion did another random shuffle and icon change and I no longer can find any of the buttons/functions that I used to use to do this. As far as I can tell, that function is no longer available, because my old models/programs lost those features. 

Specifically in regards to the mesh conversion, as I asked above, is this something that you do on a regular basis? Should I be doing this as a standard part of my "work flow"? I guess what I am asking is, how do I know when I am supposed to do this? 

I am also curious what other effects does this have? What is the balance to making these changes? If I make this change to the parent part, how else will it, could it, effect the part? Or is it more a matter of effecting the part size/computer usage? 

Thanks again to both of you for your help. 

[Steinwerks]

For this sort of work you need to dive into the Compare and Edit dialogue (right click on the toolpath) and start playing with other tolerance settings besides what the standard toolpath dialogue gives you. Changing Surface Triangulation Tolerance to tolerance*.01 instead of the default tolerance*.5 alone makes massive differences in surface quality (helps eliminate faceting for instance). Even applying it to your Parallel1 operation helps in a way seen instantly and adds virtually irrelevant generation time (2.2s vs 1.7s).