Faceted surface finish with Fusion 360 on 770

Hey everyone,

I have been chasing this down for the past few evenings, and I'm not sure if I'm trying to fix something that can't be fixed. I'm trying to machine this part:

Attachment 338352

The surface finish does not really concern me since I know I still have some speed/feed issues to resolve. What bothers me is the faceting that is going on. This is my first time working with 3 axis toolpaths in Fusion, and I can't seem to get this to smooth out. I have used ball endmills before in 2 axis operations using SprutCAM and have not had this problem. My question is is this...am I chasing a problem with Fusion that is actually a limitation of the Tormach? I plan to post this to the Fusion forums as well, but wanted to check with the Tormach owners to see what their experience is with 3 axis machining.

Thanks for taking the time to look.

Definitely not an issue with the Tormach. Here's a piece I made last night with no faceting, the marks you see are from the ball-mill cutter. I used Adobe Illustrator -> Creo -> SprutCAM for this piece.

Attachment 338372

--Bryan

Interesting. I recently machined a shallow 3D "dome" of sorts on top of a pc of hex brass stock. It was strictly for experimentation with various tool paths and to see if I could chamfer an edge curve 3D and have it come out right. Everything worked but it was faceted just like yours but even more coarse. In fact I think the dome had 6 equal sections radiating from the center out to the 6 corners. I can post a photo of it later. The model was imported directly from a Solidworks 2015 part file. I suspect there is a tolerance setting somewhere in the CAD software that may specify how small of pc's to break up curves into? The smaller you go the program size gets progressively huge. Possibly exporting as NURBS but I'm not sure how to do it or if PP can digest these.
This is an old article that may not directly solve your problem but may shed some light on the issue Interpolating Curves : Modern Machine Shop

Most of that looks like really bad chatter to me...

But, if you want help with a Fusion problem, you'll have to post the model, so we can see what toolpaths and settings you used. If you use roughing toolpath for finishing, you can get a pretty awful surface. In correct option settings can also do it. The Fusion CAM is REALLY good, so this is certainly not a limitation of FusionCAM. The 770 should also be able to produce a very good finish, it programmed correctly, though there could be something wrong with your machine.

Regards,
Ray L.

What specific tool paths are you using/tolerance settings?. Adaptive roughing tool paths will,leave facets as it is intended for roughing only. Otherwise, post your speeds/feeds/stepover etc. For 3d surfaces I usually rough at .01" steps for finishing with a 4 flute ball mill, 6000 rpm at 40 IPM and surfaces come out,real nice.

Attachment 338412Attachment 338414

Quote:

---

Originally Posted by SCzEngrgGroup

Most of that looks like really bad chatter to me...

But, if you want help with a Fusion problem, you'll have to post the model, so we can see what toolpaths and settings you used. If you use roughing toolpath for finishing, you can get a pretty awful surface. In correct option settings can also do it. The Fusion CAM is REALLY good, so this is certainly not a limitation of FusionCAM. The 770 should also be able to produce a very good finish, it programmed correctly, though there could be something wrong with your machine.

Regards,
Ray L.

---

Thanks for the replay Ray, and yes the chatter is bad...working on that as well. Here is another that I did the other night while experimenting. I cleaned up the finish a bit with some scotch brite to make it clearer what I mean:

Attachment 338452

Quote:

---

Originally Posted by AUSTINMACHINING

What specific tool paths are you using/tolerance settings?. Adaptive roughing tool paths will,leave facets as it is intended for roughing only. Otherwise, post your speeds/feeds/stepover etc. For 3d surfaces I usually rough at .01" steps for finishing with a 4 flute ball mill, 6000 rpm at 40 IPM and surfaces come out,real nice.

---

I'll upload the file tonight (if possible) when I get home. For that pocket, I'm using a 3/16" 2-flute ball endmill to first do a 3D Adaptive clearing leaving .010" for cleanup. Then I am doing a scallop as the finish with a .010" stepover. I thought scallop was a finishing pass...am I mistaken? Currently, the only 4-flute that I have that would fit is an 1/8". I was going to try that to see if it cleans up the finish, but I don't think it will do anything for the faceted finish that I'm getting.

I thought the lines were being left behind by the 3D adaptive routine, and that I wasn't leaving enough material for the finish to eliminate them. But I ran it again, and it's very noticeable in the table movement that the lines are being introduced during the scallop. Very jerky table motion. I don't think there is anything wrong with the machine though since other circular paths are extremely smooth.

I'll put together a more thorough post with better information tonight.

How big is that part? 3/16" and 1/8" are mighty small tools for what looks like a ~6" diameter part? If so, you should be roughing with something more like a 1/2", finishing with something between 1/4" and 1/2", and using the small tools only for getting into the corners and other features that are too small for the larger tools. Scallop is not the best path to use for that either. I'd use 3D contour.

I'll be out tonight, but if you post the Fusion model, I'll take a look at it tomorrow.

Regards,
Ray L.

Quote:

---

Originally Posted by SCzEngrgGroup

How big is that part?

Regards,
Ray L.

---

Hi Ray,

In the very first picture I posted, the stock is 2.5" square by .75" thick with .010" stock on top before machining. I'll try a 3D contour path tonight to test.

Juan

Quote:

---

Originally Posted by C*H*U*D

Hi Ray,

In the very first picture I posted, the stock is 2.5" square by .75" thick with .010" stock on top before machining. I'll try a 3D contour path tonight to test.

Juan

---

Oh! Much smaller than it appeared. So maybe rough with 1/4", finish with 3/16" and/or 1/8". How much material were you removing on the finish pass? What RPM/feed/stepover? The finish suggests you were getting butt-loads of tool flex, which means your feeds and speeds were likely way off, or you were trying to remove too much material.

Regards,
Ray L.

General rule of thumb: use the largest cutter that your part will support (up to 1/2" anyway). Seems like you could easily fit a 3/8" or bigger endmill into that part.

1. How much stick-out do you have on the endmill?
2. How are you calculating feeds and speeds for your cutters? What values were you using?
3. How are you securing the part you are cutting to the table?

How about you run a circular pocket in a chunk of aluminum using path pilot conversational mode, and see if it gives you the same finish? That could tell you if it is a CAM or a machine problem.

I found out some interesting things today. I made some changes when posting this last run

Attachment 338574

The faceting is still there but not as bad. Or it may just because of a slightly better surface finish...still working on that. Again, this is still using the Scallop path. I still want to experiment with others, but would rather not change too many things at once.

Attachment 338576

So then I decided to try Morphed Spiral. Everything else is the same but the faceting around the circular path is totally gone.

Attachment 338578

Now this is the interesting part. When I zoom in on the Scallop tool path in Fusion, it's very jagged. At first I just thought it was a graphics setting somwhere to help with framrate:

Attachment 338580

But, the very same position showing the Morphed Spiral doesn't have this graphics issue:

Attachment 338582

So this tells me that Fusion really is posting that Scallop path just as it looks. Sorry this turned into a Fusion post...I just wanted to confirm it wasn't the 770's fault before I chased down a problem that didn't exist.

Thanks to everyone who took the time to take a look and reply.

Juan

Use a square endmill for your roughing passes and save the ball nose for your finishing path.Remember that the effective SFM at the tip of a ball nose approaches 0.

bob

Juan,

What have you set the Tolerance to on the spiral?

This is a screen shot of the tolerance setting.

Attachment 354290

Have you checked the smoothing box? I think this attempts to use arcs instead of straight lines in the G-code ("I think" being key here) but it smooths out faceting on contours without cranking tolerance to crazy levels. I usually set tolerance and arcs to 0.001".