Possible bug with CAM gcode output.

[Anonymous]

Hello fellow Fusion Cam fans,

I have been using fusion 360 for a while now and am starting to get used to it. I love the Fact that It is an all in one software, from sketch to 3d design to cam and then Gcode. I have a small CNC Mill that I machine mainly soft plastics, glassfiber sheets and wood. I used to use freecad and a programm called CAMBAM to do my designs and make the Gcode. I have been doing it like this for a few years now and everything worked fine, It was just a long process.

Recently I have designed a part in Fusion 360, a new hoover fiting for the mill. Through the CAM tab in fusion made the requred toolpaths and outputed the gcode using the "mach3mill.cps" postprocessor. I ran some simulations before and it all seemed fine.

Now comes the problem....

The Cam tab has 4 process's, 3 cut fine but on the 4th it starts to drift on the y axis.

1. A slot around the outer edge.(2mm endmill)

2. 4 Holes for magnets.(6mm endmill)

3. 2 large holes. (6mm endmill)

4. The outer shape. (6mm endmill and Here's the problem)

It appears to drift upwards on the y axis by about 1mm on each pass around the outer edge. I have ruled out backlash and am 99% sure that its not missing steps. (If it is missing steps its doing it in exactly the same places, Everytime I run the code and only on the last toolpath.... VERY unlikey) It is as if it happens gradually over the course of one time around, There is at no point a recognizable "step". What I dont understand is why it can cut everything else fine but not the outside cut, In my opinion it has to be a software/ gcode problem.

I have also tried a few different things like:

- Plunge into matirial and ramp into material

- With and without lead-in and lead-out.

- Changing the cutting feed rate.

.... But the result was the same everytime.

I must admit that fusion can do alot more than what I understand sometimes, maybe I have missed something but I am currently at a loss and don't know what else I could try.???? Any help would be Greatly appreciated!

Here is a link to the model im trying to cut: http://a360.co/2dtOIje

... And I have attached some pictures to show the result after cutting (I didn't let it run until the end as i could see it wasn't correct)

Luke

[Anonymous]

...And here is the .f3d file

[RandyKopf]

I just want to ask a really silly question... Are you sure the spindle is running in the right direction? It looks like the material is being pushed or melted? What is the material by the way? Is that material Polypropylene? Cause that stuff does not like to be machined at all. And you would need decent clamps just to hold it. Is it possible the spindle rpm is too fast? I just don't see evidence of clean cuts and chips. Looking at the attached model in A360 the CAM tool path plays like it should. I can't open it in Fusion from work. It looks like the part is being moved like it is resisting cutting.

[Anonymous]

Yes spindle is running correctly, the matirial is Pom-c plastic. Its a bit of a pain to cut, but im sure that has nothing to do with it as the rest cuts fine.

[RandyKopf]

Is the part being moved out of position? What spindle rpm and feed rate are you running that at?

[Anonymous]

no the part is solid it cant move.

My spindle speed is 11500 rpm and feed rate is set to 800. I have used these settings many times for cutting this plastic and it works fine.

[xander.luciano]

Hello!

Can you post the NC code you ran also?

Thanks,

[Anonymous]

for some reason it wont let me upload a file with a .tap extension????

[xander.luciano]

Hey,

Just rename it to .NC or .txt then.

Thanks,

[Anonymous]

.... i should have thought of that. 🙂

[HughesTooling]

Here's a backplot of your code and there's no problem there. What happens if you go back to one of the holes, can you jog to where they should be and see if the machine setup is still correct. 

You can download a good backplotter here NC Corretor.

Mark

[xander.luciano]

Hello!

G code looks fine on my side also, but looks like you are getting some part movement or vibration as it's being cut, also appears that you have lost your tabs

Also, I would recommend doing boring operations instead of pockets for the 4 smaller holes. The 1mm stepdown is pretty shallow for a 6mm cutter also, You could likely bump that up to 3mm even for a full WOC. 

The melted plastic is on the side where the material to cut is thinnest, but also where it needs to evacuate from, so every revolution a chip is being rubbed up against that exterior wall causing heat and friction, which is probably the source of the melting. I think you should decrease the spindle speed so that it creates bigger chips which should help remove some of the heat (plastic is insulting so it won't absorb as much heat as a metal chip). I think you just need to be a little more aggressive with the cutting to reduce the heat some. The fact that it is insulting also means more heat is going to stay in the endmill, causing it to just melt through the plastic and displace it on the outer edge instead of truly cutting the material.

Hope that helps some! Let me know how it goes on the next run,

Best,

[RandyKopf]

So something is not right here... I've cut several plastics but missing something here... So in my humble opinion the machining is not cutting but melting. Something is way off in this. Perhaps this is of a scale that is not typical to what you do. The photos speak for themselves. Just as Xander.Luciano pointed out there likely is a problem with chip evacuation. It explains why everything is off. There is way too much heat staying in the cut path. And that is jacking up your intent. It's not a Fusion CAM problem per se doing this but it's more about the setup. It's solvable, maybe the tool is not ideal for this cut type. A 4 flute tool could cause this. Or even a tool designed for finish of composites would give this result. I suggest a single flute "Up Shear" router bit for chip evacuation as that would be ideal. http://ballewsaw.com/onsrud-63-701-single-flute-sc-upcut-spiral-o-flute.html?___store=default&gclid=... Perhaps slowing the feed rate down would help. Maybe cooling the cut with compressed vector air like a cold air gun. http://www.exair.com/en-US/Primary%20Navigation/Products/Cold%20Gun%20Aircoolant%20Systems/Pages/Col... Well that is what I am seeing and that is where I would start. I am no expert in this. Well this is my 39th year in manufacturing and I don't know jack squat. But hoping to meet him one day haha. In the mean time I may be old but try to get the advice of those near me to help me get it a bit closer to being right. I sincerely hope this helps.

[Anonymous]

Firstly thanks to everyone for their time and help!!

I have just done a dry run.... Spindle off, cutting in the air above the stock. My goal was to see if poor cutting was affecting the positioning and to see if the machine returns to zero once done. It completed the gcode and then I told it to return to zero and it was off by ~10.5mm on the y axis.

This tells me two things:

1. The code is fine (As you allready knew)

2. The problem has nothing to do with the actual cutting, (melting the plastic instead of cutting).

The problem now in my eyes is the machine itself or in Mach3 software, The strange thing about that is that the machine has been working great for the past few years, the only thing I have changed is the way i make the code. (Now in fusion, before in CamBam)

Are there any Mach3 users out there that have any ideas?

[HughesTooling]

@daniel_lyall might be able to help. Also don't rule out coincidences, the universe loves to have us running in circles, can you program the part in CAMBAM and see if it gives trouble. Does CAMBAM use G02/03 and helical moves? I've got a mach3 control on a small engraving machine and it works fine so I'm not sure there's anything in the code that's causing the problem.

Mark

[xander.luciano]

Sounds like we're getting closer to nailing down the true issue here! This community is really active and there are lots of knowledgeable guys here that are happy to offer up their advice so I'm certain we'll get this cutting correctly for you! 🙂

When you say "It completed the gcode and then I told it to return to zero and it was off by ~10.5mm on the y axis."

How did you do this? Do you mean that you ran the code then manually told it to do this: "G54 G00 X0.0 Y0.0" Or did you do a G28? How did you measure the difference? Did you look at the reported position or did you physically measure from a known location? E.g. G00 X0.0 Y0.0 and your machine was ~10.5mm away from the point you used as your WCS

This is a strange issue to have occur because this would have happened no matter what program you posted code with (makes me think that maybe the steps/revolution is off). Maybe test this by putting the machine some location Y, putting something there to just hold the position, then "G91 G00 Y-1.0" (or "G91 Y1.0") maybe 6 times, then do "G91 G00 Y6.0" and see if it ends up in the same spot. That should tell you if the error is machine side. 

Lastly, "the only thing I have changed is the way i make the code."
This makes me think that possibly there is a difference in the code being posted. If you can provide a known working NC file I'm happy to compare them and see if there are any differences. I'm mainly interested in seeing if G2 and G3 are the same for both.

If it ends up being the post processor, I'll happily make the changes and get you a new version! Can you also tell me what control and version you are using (or maybe a manual for it?). 

We'll just have to slowly eliminate possibilities until we find the source of this issue!

Best,
Xander Luciano

After thought! - Post just the last operation (2D Contour 4) and dry run that, see if you get drift in the Y axis.

[Anonymous]

I ran the code then used the button in mach3 "return to zero" this returns the cutter to the point where it was zeroed to on the stock to be cut. From there I could see that it wasn't in the same place, I crudely measured it with a dial caliper. Mach3 was showing the position to be zero but in reality it was about 10.5.

If the steps/revolution was off then surely the circles that it cuts first in the code wouldn't be perfectly round.... but they are. It cuts everything else fine, just the outside profile is creating this problem.

I have already tried posting just the 4th profile and the result was the same.

I have attached a Gcode file that I know works fine, It was made with cambam.

Thanks for all the help guys!!!

[daniel_lyall]

@Anonymous

First if a axis is off by any amount check all mechanical parts, that the first thing you need to do.

then check all electrical connections every single one.

what version of Mach3 are you useing??

What type off machine is it ??

what controller are you useing??

then check to see if the machine is Squire.  draw a line in X then Y and lay a squire along the X line if the Y line lines up it's squire if not that needs fixed. stick a pencil in the spindle to do it.

@HughesTooling sounds mechanical, or Mach has gone nanana it can do that from time to time

[Anonymous]

The machine mechanics are from ebay, they called it a "6040". When I recieved it i took it all apart and put it together "properly". The electronic side of the machine I have done myself, It uses separate stepper motor controllers and a parallel port breakout. It Is not a off the shelf solution but it has proven to work fine the past few years.

Im not at the machine right now so I can't say what version of mach it is, but i can say that its not a recent version. I don't mean to put your advise down but this surely has to be a software problem, It cuts other things fine just the outer profile on this part is creating this problem.

when im at the machine tomorrow ill give it a good check to see if I can find anything, but I doubt I will.

[HughesTooling]

One difference in the code is CamBam is using IJ arc centres and the default using Fusion's mach post is R. It shouldn't make any difference but can you test again and on the post dialog set useRadius to no.

Mark