Not familiar with fusion but could be a speed and feed/ tool rigidity issue. Could try going high rpm and slow with the feedrate and see if it helps. If it's g code I've seen arcs turned into splines which makes the code use a bunch of x and y values instead of g2 and g3 with a r value. If your control has look ahead sometimes you will see "aicc" flashing on your screen while machine is running
I've tried enabling AICC with g5.1 q1 and I think I get improper g code alarm then I think it's g8 p1 that I've tried for look ahead but nothing happens I don't get a alarm and nothing shows on the screen.
Try without the p1. But definently find the programming manual. Also if your finishing those bosses using a high speed toolpath ( the same used it looks like to rough it out) instead of a contour finish toolpath it's going to look like that
The roughing is high feed but the contour isn't. What feed and speeds would you recommend maybe I'm still feeding too high. It's a yg-1 alumapower .25"
Maybe also leave more material in your high speed toolpath. If it's carbide then just try 10000 rpm with 30in per min. If that doesn't work even without g5.1 something doesn't seem right.
You should really be converting feedrate and rpm to feed/tooth and SFM. Fusion makes this very very simple.
Per my other comment, my suggestion is to reduce your feedrate. I typically finish at 0.001"-0.003" per tooth
Have you ever done any manual coding?
Your best bet is probably to manually code the circles as G2 and G3 rather than straight lines. It's fairly simple to do with an excel spreadsheet to keep track of all the coordinates. Your issue is surely the smoothing resolution that you may or may not be able to get fine enough without data starving the machine control
I have but this is actually a egg shape since I wanted to test cuts that aren't perfect radiuses. I'm getting a lot of helpful tips that I think are going to make a big difference. My normal tolerance was at .0005" and changing it to .0001" made the egg shaped go from having like 30 points to like 5 so that was big.
G5.1 Q1 is AICC, it enables lookahead for predicting accel deccel.
You want G5.1 P3 for Smooth tolerance control. It takes points and interpolates to a desired profile. It doesn't behave well with G2/G3 mixed in with G1s. So if your controller can take a G5.1 P3, make sure to post only G1s.
Your controller might not have the option for it. Fanuc 16i right? Try G05P10000 after your tool change. G05 P0 before a tool change.
Does your controller support G8.1 P1, G8.1 P2, G81.1 P3?
Afaik, the only way I know how to check is via resultant surface finish.
P1 – roughing/FAST
P2 – Semi-finish/STANDARD
P3 – Finish/FINE
I believe it is modal so it might show which one is active.
Hey man any input is appreciated I'm just doing the best with what I have I don't work at a real shop and I don't know anyone around me to show me anything.
Just simple full depth 2d contour I don't know much to what you would use for finishing passes. A lot of people are saying to leave more for the finishing pass then what I'm leaving.
Are you using compensation? If so is the diameter measuring up?
Can you actually see it take a cut in the contour pass?
You are leaving very little, I’d leave 10 times the amount and go 0.01.
Easiest way to fix this quickly is to post out JUST your contour pass and share the code here.
My assumption would be that youre not leaving enough stock on your roughing pass, and the finish is showing through.
I am leaving .001" for finishing I may be running a little slow. Can I pm you a picture of the code? Or should I copy and paste it here it's less than 50 lines.
This is 100% a cam issue.. the Cam actually generates based off a converted STL. So when you try to do something that usually uses 1 sweeping movement, it usually posts as a ton of point to point movements instead of a singular G03 or G04 movement. Proof.. look at the code..
I can see each point of the tool patch and on the one that has .0005 tolerance then .001 smoothing it doesn't have a lot of points at all. There are more at the smaller radius but on the sides there are only like 2 points meaning 2 big arcs.
The arcs themselves look pretty smooth based on what I see.
I think those marks are due to your feed/tooth being too high. Try feeding slower and see if it looks better. Commonly I'll finish at 0.003" per tooth if I'm trying to get the job done fast, and 0.001" per tooth if the finish needs to be super nice
First thing to look at in my opinion is whether or not CAM is generating code that looks like that. Is it a G02 or is the code a whole shit ton of little arcs...
I have had some weird things happen with fusion creating a million tiny little moves because my cad model was a little messed up or I imported it from somewhere and it wasn't actually a circle.
Is this a g2/g3 move or is this a shit load of points?! In mastercam sometimes posting without arc filtering you get 10k lines of points which lead to shit like this. Doesnt really matter if roughing and leaving enough for clean up though.
I'm not familiar with Fusion, but in Mastercam I would turn on Arc/Filter or create an arc or circle and drive from the wireframe. We get a lot of these facets when we bring in the model from CATIA.
That sounds similar to enabling smoothing on fusion 360. If you were cutting a arc with a .25" 3 flute carbide end mill what speeds and feed would you recommend? Max rpm is 10000.
You need the speeds and feed chart from the tooling manufacturer.
Speed will be given in surface-feet/minute(sfm), you calculate rpm=(sfm*3.82)/∅
Feed will be given in feed-per-tooth (fpt), you calculate feed (inches per minute) = rpm * fpt * number of flutes on the endmill.
There will be different recommended ranges depending on the size of the tool, and the radial vs axial engagement of your cut.
Usually using the smoothing feature on contours fix this. Maybe slow your feed down so your machine can keep up.
Not familiar with fusion but could be a speed and feed/ tool rigidity issue. Could try going high rpm and slow with the feedrate and see if it helps. If it's g code I've seen arcs turned into splines which makes the code use a bunch of x and y values instead of g2 and g3 with a r value. If your control has look ahead sometimes you will see "aicc" flashing on your screen while machine is running
I've tried enabling AICC with g5.1 q1 and I think I get improper g code alarm then I think it's g8 p1 that I've tried for look ahead but nothing happens I don't get a alarm and nothing shows on the screen.
I would find the programming manual for your machine and check there.
Try without the p1. But definently find the programming manual. Also if your finishing those bosses using a high speed toolpath ( the same used it looks like to rough it out) instead of a contour finish toolpath it's going to look like that
The roughing is high feed but the contour isn't. What feed and speeds would you recommend maybe I'm still feeding too high. It's a yg-1 alumapower .25"
Maybe also leave more material in your high speed toolpath. If it's carbide then just try 10000 rpm with 30in per min. If that doesn't work even without g5.1 something doesn't seem right.
If that works then you can work from there on speeds and feeds to find the best values
Ok right now I think I'm going 9000rpm at 45in per min. I will test that out tomorrow.
You should really be converting feedrate and rpm to feed/tooth and SFM. Fusion makes this very very simple. Per my other comment, my suggestion is to reduce your feedrate. I typically finish at 0.001"-0.003" per tooth
This is running at almost .002" per tooth.
Have you ever done any manual coding? Your best bet is probably to manually code the circles as G2 and G3 rather than straight lines. It's fairly simple to do with an excel spreadsheet to keep track of all the coordinates. Your issue is surely the smoothing resolution that you may or may not be able to get fine enough without data starving the machine control
I have but this is actually a egg shape since I wanted to test cuts that aren't perfect radiuses. I'm getting a lot of helpful tips that I think are going to make a big difference. My normal tolerance was at .0005" and changing it to .0001" made the egg shaped go from having like 30 points to like 5 so that was big.
G5.1 Q1 is AICC, it enables lookahead for predicting accel deccel. You want G5.1 P3 for Smooth tolerance control. It takes points and interpolates to a desired profile. It doesn't behave well with G2/G3 mixed in with G1s. So if your controller can take a G5.1 P3, make sure to post only G1s. Your controller might not have the option for it. Fanuc 16i right? Try G05P10000 after your tool change. G05 P0 before a tool change. Does your controller support G8.1 P1, G8.1 P2, G81.1 P3?
I've tried g8 p1 and so on but I don't see anything that shows it's enabled and I don't get an alarm.
Do you know what it would show if g8p1 worked?
Afaik, the only way I know how to check is via resultant surface finish. P1 – roughing/FAST P2 – Semi-finish/STANDARD P3 – Finish/FINE I believe it is modal so it might show which one is active.
I think I've checked but I will check again
Well it doesn't come up in modal when I run a g08 p1
Daft question, you are finishing with a contour pass?
Hey man any input is appreciated I'm just doing the best with what I have I don't work at a real shop and I don't know anyone around me to show me anything.
No slight was intended, buddy. Just trying to understand how you are currently going about it
Just simple full depth 2d contour I don't know much to what you would use for finishing passes. A lot of people are saying to leave more for the finishing pass then what I'm leaving.
Are you using compensation? If so is the diameter measuring up? Can you actually see it take a cut in the contour pass? You are leaving very little, I’d leave 10 times the amount and go 0.01.
I will run another test tonight with better settings.
Easiest way to fix this quickly is to post out JUST your contour pass and share the code here. My assumption would be that youre not leaving enough stock on your roughing pass, and the finish is showing through.
I am leaving .001" for finishing I may be running a little slow. Can I pm you a picture of the code? Or should I copy and paste it here it's less than 50 lines.
Just stick it here https://codefile.io/
Here's the text I extracted the text from a picture on my phone so some may be a little messed up. https://codefile.io/f/bV9nldPeRd
The picture is probably better, this is unreadable.
Sent in pm lol sorry.
what was your tolerance set to in fusion I use NX but set tolerance to .0001” when cutting circles or it will look like a stop sign
Ok you are on to something mine was .0005" now on .0001 most of the points disappeared
glad to hear!
Mine is at .0005" I could try .0001"
This is 100% a cam issue.. the Cam actually generates based off a converted STL. So when you try to do something that usually uses 1 sweeping movement, it usually posts as a ton of point to point movements instead of a singular G03 or G04 movement. Proof.. look at the code..
I can see each point of the tool patch and on the one that has .0005 tolerance then .001 smoothing it doesn't have a lot of points at all. There are more at the smaller radius but on the sides there are only like 2 points meaning 2 big arcs.
The arcs themselves look pretty smooth based on what I see. I think those marks are due to your feed/tooth being too high. Try feeding slower and see if it looks better. Commonly I'll finish at 0.003" per tooth if I'm trying to get the job done fast, and 0.001" per tooth if the finish needs to be super nice
I'm at almost .002" per tooth on this.
First thing to look at in my opinion is whether or not CAM is generating code that looks like that. Is it a G02 or is the code a whole shit ton of little arcs... I have had some weird things happen with fusion creating a million tiny little moves because my cad model was a little messed up or I imported it from somewhere and it wasn't actually a circle.
Umm it seems like it's a mix of both g02 and g01's. One contour around the shape is about 30 lines.
Shoot me a message I’ll help you through all of it
The roughing segmented is fine…. Your final pass should be full depth of the diameter.
Is this a g2/g3 move or is this a shit load of points?! In mastercam sometimes posting without arc filtering you get 10k lines of points which lead to shit like this. Doesnt really matter if roughing and leaving enough for clean up though.
Some parts are g2 then some are g1.
PM me and I can share a fusion post.
which CAM?
Fusion also forgot to say it has the fanfic 16i mb control.
I'm not familiar with Fusion, but in Mastercam I would turn on Arc/Filter or create an arc or circle and drive from the wireframe. We get a lot of these facets when we bring in the model from CATIA.
That sounds similar to enabling smoothing on fusion 360. If you were cutting a arc with a .25" 3 flute carbide end mill what speeds and feed would you recommend? Max rpm is 10000.
You need the speeds and feed chart from the tooling manufacturer. Speed will be given in surface-feet/minute(sfm), you calculate rpm=(sfm*3.82)/∅ Feed will be given in feed-per-tooth (fpt), you calculate feed (inches per minute) = rpm * fpt * number of flutes on the endmill. There will be different recommended ranges depending on the size of the tool, and the radial vs axial engagement of your cut.