Better 5 Axis CAM software?

[erics...@gmail.com]

What are people using to create 5 axis GCode? I've been muddling through with Fusion 360, and while I'm making some headway, it's obvious that this is a workflow of workarounds more than easily creating toolpaths because Fusion is meant for 3 axis only.

Has anyone been able to get any actual 5 axis software working? I saw a mention that there might be a post processor for MasterCam...

I also came across this:

http://www.cnc-toolkit.com/

I'm going to be giving that a try...

[Xander Luciano]

Hello!

When you say "this is a workflow of workarounds" What do you mean? I find programming 3+2 inside fusion to be extremely straightforward and simple to use. One of the better programs I would say. What problems are you running into? And what type of parts are you trying to program?

Best

-Xander Luciano

[erics...@gmail.com]

I'm trying to setup some toolpaths for a bust of a head. It's working, but having to make all of these planes, and the containment boxes is a lot of work. The end result is a toolpath that has to stop and start. If I could do true 5 axis milling I could have the move the A and B axis continuously as I mill around the bust. That would give the best finish.

So this method does work, and it's probably the best way to go about it now.. However it seems that it would be easier if you could do more (more easily) than 3+2 if you had a program that was more suited for this machine.

[Randy Kopf]

Eric:

You won't be able to do this with Fusion 360 at this time. Fusion supports 3+2 machining. 

I bought http://www.deskproto.com/products/multiax-ed.php hobby license for $299. It's not a true full 5 Axis software but it does tool paths that Fusion can't. I have a post that is working for Pocket NC for a specific application for Ring machining. it will work for the bust example.

Desk Proto is a very fast easy to generate NC code. It's not written for machinists but for people just wanting to cut parts.

I am in process of working on a 5 Axis type mode in Desk Proto at the moment. I have not tested the post across all the possible configurations of Desk Proto. 

You can see an example of DeskProto cutting my parts here.

https://drive.google.com/open?id=0BxziiLimgn9SX25Ed1J0QWl2cTQ

And another finish cut method here

https://drive.google.com/open?id=0BxziiLimgn9SbS1nSUoxa0lJZDA

You can also see the end results on my blog listed below.

Randy

http://desktopartisan.blogspot.com/

[erics...@gmail.com]

That looks great!

I just realized that I have Inventor HSM which has 5 axis capability. I've started fooling with it and it's a lot like Fusion, but it seems to have more features.

I'm seeing if I can mill that bust using a turning toolpath....

[erics...@gmail.com]

It looks like there's no Pocket NC post processor for Inventor though.. I wonder if the Fusion one could somehow work?

[Randy Kopf]

Eric:

The Pocket NC post will work with Inventor HSM. All the Autodesk CAM products posts are inter changable. Just copy the Pocket nc post it's got a .cps extension to the HSM Post directory. 

The tool paths will look and act pretty much identical. And yes HSM Works has the early 

There is help on the HSM side getting the post in the right place ask for input here:

http://forums.autodesk.com/t5/post-processors/bd-p/218

Randy Kopf

http://desktopartisan.blogspot.com/

[erics...@gmail.com]

Alright, I've had another go at this and it's incredibly frustrating....

I've watched the 3 part impeller tutorial way too many times and I haven't gotten it to work properly. The fact that you have to have all those planes and containment boundaries makes it rife with the possibility for errors. Plus, with a 5 axis machine I'd think you should be able to spin that plate around continuously to make something like this.

In an attempt to simplify I tried doing one simple single 3 axis toolpath with Fusion. I couldn't get that to work because I was thwarted by not being able to actually save my tool path (despite me following exactly the way it was done in the video)

So now that I realized that I have Inventor CAM (that is 5 axis) I thought that might be a better option. I found the interface to be nearly identical to Fusion. I got started with setting up toolpaths and I was able to make them more easily.

I was also able to save them directly to the machine. This was either because I am now using Inventor, or because I was doing it through windows. Either way, this is as far as I could get:

https://www.evernote.com/l/AC43bPER0JVOQ7NP7yaW06BQBt3TgtGh0x4

I think the problem here is that my Z offset isn't correct... Despite me trying to adjust it several times I cannot get it to work right.

I'm no stranger to CNC machines, I built my own years ago and I operate two daily. Granted they are all 3 axis.

I've had this machine for a couple of weeks now and I cannot get it to do anything meaningful, not even cut or move in any basic way outside of jogging it around.

I think what you guys need are some more basic tutorials. Maybe just a few that show how to cut in 3 axis, then 4, then 5. Maybe some basic ones where you create a super basic toolpath just to get the machine moving.

Right now I feel like it's an impossible uphill battle with the software. I hope you don't take my comments here as negative. I think this machine is incredible and I'd love to help make it easier for people to use it...

[erics...@gmail.com]

Ok, another update:

I was able to figure out a workaround to get my saved GCode in the proper format from my computer to the PocketNC. The Gcode is now readable.

I can get some decent looking toolpaths out of Inventor, but when previewed on on Linux CNC they all appear to be above the Z axis, not below it. Despite me attempting to flip the Z I cannot get this to work...

I am still unable to make any toolpaths generated from Fusion to do anything at all.

Any help would be greatly appreciated!!

[Michael]

Hey Eric,

I was wondering if your post processor may be giving you some bugs. 

The start of your code should look like what is posted below.

one area i have been working on adjusting in a different post processor is making sure that the height offset of the tool is loaded properly. It shows up on N85 where the first Z axis move is done. If this value isn't entered the machine will just use the home location for the machine and won't offset the tool to its defined location. This may be what is causing the tool to stay way higher than normal. 

N10 G20

N15 G90 G94 G40 G17 G91.1

N20 G53 G0 Z0.

(2D ADAPTIVE2)

N25 M9

N30 G49

N35 M5

N40 G53 G0 X2.5 Y2.5

N45 M0

N50 T10 M6                          Tool called up and loaded

(SINGLE FLUTE)

N55 S8500 M3

N60 G54 G0

N65 A90. B0.

N70 M9

N80 G0 X-0.7581 Y-0.8635

N85 G43 Z1.32 H10                       Tool height offset

N90 G0 Z0.89

You can check to make sure your offsets are correct by running your code and after the machine has moved the z axis towards the material your should see in the user interface that the Tool is loaded (this shows up right at the bottom of the screen "Tool 10, offset -2.591, diameter 0.125"). You should also see that the Tool length offset (TLO) is defined up in the bottom part of the DRO part of the interface. It will show that the TLO Z offset is -2.591 in this case. Check out the picture attached to see these values. In your case these values will likely be different depending on your tool length offset.

Let me know if this helps,

Michael

[Xander Luciano]

Eric,

Fell free to post the code you are generating and maybe a screenshot of axis as well so we can help trouble shoot and see where the issue lies!

Best,

-Xander Luciano

[erics...@gmail.com]

Sorry for the silence folks, I've made some progress:

https://www.facebook.com/greenfieldmakerspace/videos/467953203398141/

THAT is a 5 axis toolpath that I generated from Inventor.

Let me backtrack though... If you've looked on this forum you'll see that I've had many issues getting started with this machine. To make this easier let's start with my connectivity issues:

The trouble I had getting connected was totally alleviated by attaching my own monitor and keyboard to this machine. If you're having trouble with connectivity, check the other threads, there are some great posts about getting connected. Once you get past that there are lots of "gotchyas" along the way that tripped me up. I'll do my best to clear these up:

First, this is a 5 axis machine. I thought right out of the gate it would be easy to make toolpaths for 5 axis. Turns out it's not.

You have to think 3 axis machine, but you're able to turn the fixture any way you want. This makes the machine really flexible, but it's a different way of thinking about toolpaths. It's not one crazy toolpath to mill your whole part, it's many that work together in different orientations.

I went through the impeller tutorial and tried to replicate it. Every damn time I made even the most basic toolpath and saved it to my machine I got errors that the code was going to make the machine move outside it's envelope. I endlessly messed with my toolpaths to try and get it to work.

The best result I was able to produce was a lone circle.

Thanks to some outside help, I got a great tutorial and I nailed it. I had setup my tool offsets, but I did it totally wrong. This machine's offsets are vastly different than my 3 axis machines. Look at the tooloffset help on the Pocket NC website. That will help you.

The other thing that got me really screwed up was creating the toolpaths. Because I had my tool offsets wrong none of my toolpaths were working. I endlessly flipped the axes of my models and toolpaths to try and get something to work.

Once I got my tool offsets working some of my toolpaths started to work. It was then I was able to dial in a method of creating reliable toolpaths that I could test.

Paying really close attention to the orientation of the fixture model, and the orientation of your toolpaths is really critical. Once you get the hang of it you'll start to be able see how you can orientate them the right way.

I am by no means an expert, but I now am heading in the right direction. I think this machine is awesome and I cannot way to start creating some great stuff with it.

[Randy Kopf]

Eric:

Nice progress!!! Now make that tool path move all 5 axis simultaneously, Maybe A was moving while XYZ and B were but it wasn't obvious.

I liked your comments. 

Thinking like 3 axis plus rotating the part is actually 3+2 and it's actually huge.

True 5 Axis tool path takes the right part to even benefit from it.

Maybe a ring with text all around it is a good example. if the ring is not actually a simple band.

Anyways regardless congratulations of figuring some things out.

Wishing to see you measure that air part next haha

Randy

[Bryanbdp p]

Erics, what type of monitor did you hookup? I tried a VGA with adapter to HDMI that I use with Raspberry Pi's, but it didn't work with the PNC.
Are you using a DVI with adapter?
Do you have to do anything special to add the keyboard/mouse/monitor, or does it just boot right up?
Thanks,
Bryan

[erics...@gmail.com]

Thanks Randy! I don't have close to anything figured out just yet, but I do feel like I'm heading in the right direction.

It was hard to see in the video, but I was milling a circle in mid air at a 45 degree angle. I tipped the circle a bit so that I could get the A axis to move a little. The limitation with Fusion is that it's only 3 axis. Inventor is 5 axis, but it can only follow one contour around an object, it can't "wrap" any milling operation around the A or B axis. So it's something, but it's not exactly useful for things I'd like to accomplish with this machine.

With these limitations (or just MY limitations) with the software wrapping the text around a ring might be impossible in one toolpath right now. I have started attempting to do a turning toolpath. Perhaps I could spin the B axis with a ball nose bit and carve out 3D shapes like that.

Bryan:

I used a computer monitor that has dedicated HDMI input. I connected a standard HDMI cable between the PocketNC and the screen. For the mouse and keyboard I used a USB setup. I plugged in a hub since the PocketNC only has one USB port.

The only caveat is that you have to plug the hub in when the machine is powered off. It can't already be on or it won't recognize the hub.

Two things to try:

Power the pocket NC totally off. (Even unplug it's USB cord if you have it connected to your computer)

Connect your screen, keyboard and mouse and power it back up. Wait a little bit. My screen doesn't come on right away. It takes a little time (maybe under a minute) before you start seeing anything.

[Randy Kopf]

Eric:

I've got a couple Fusion 360 CAM files I could send your way if you like.

One uses A90 rotated and does some text.

The other does a compound angle and cuts a surface. It uses a NC Pattern and repeats that but rotates B30 degree cuts the surface again and repeats with the B60 etc... until the entire part is cut.

And least you can see the setup...

Randy

[erics...@gmail.com]

That would be awesome! I'd love to see those!

[Randy Kopf]

Eric:

Sorry for the delay... I just created a post that hopefully will help you and others...

Click here to go to that post

or copy and paste the following link into a web browser...

https://groups.google.com/forum/#!topic/pocket-nc/anfiQrBirvU

Hope the files help...

Randy Kopf

http://desktopartisan.blogspot.com/

[erics...@gmail.com]

https://goo.gl/photos/g6gyJ4sbtWWsSv4a6

Working nicely!!

[Randy Kopf]

Eric:

Very Nice!!!

Randy Kopf

http://desktopartisan.blogspot.com/