topic Re: Setting up Fusion for mill's limits and outputs. in Fusion Manufacture Forum

Setting up Fusion for mill's limits and outputs.

Anonymous — Tue, 18 Apr 2017 16:01:16 GMT

Hi - New to CNC milling, Fusion 360 and the forum and need to figure out the basic setup for my machine. I have a System M3X and was suggested to use the Generic Fanuc post processor. Here are the issues I am running into:

When running the program, the machine's limits are hit and it won't go to the next step without making manual adjustments (limits exceeded warning). How can I set the limit's within fusion to stop this from happening?
I am learning to use G-Wizard for the feeds and speeds, but how do I translate that into all the other variables within fusion concerning the tool's lead in feed rate, lead out, ramp, plunge feeds, etc.? I think it was suggested to use the same feedrate for all of them to start, but I could have misunderstood.
Is there a way to set the tool holder's within Fusion, concerning the tool number? The program chose to use T9 and T8 for the initial tools, and I would like to use tools 1 & 2 instead.

As I mentioned, I am learning quickly (for me), but am very new to the CNC world. I am setting up to produce a few parts of my own for small production and any help is greatly appreciated!

Thank you,

Billy

Re: Setting up Fusion for mill's limits and outputs.

LibertyMachine — Tue, 18 Apr 2017 16:17:23 GMT

1) Does it alarm out right off the bat, or is it sometime later on in the program? If it's right away, I'd be suspecting the G28 move at the beginning. Does your machine have limit switches?

No, you cannot set the limits inside of Fusion, really. All you can do is make sure your WCS setup is correct. Meaning, where you set your zero in Fusion is the same spot on the machine, and at the machine; make sure you have enough travel. More info in this area would be helpful for us to advise you better

2) It depends on operation, material, HP, tooling, coolant, rigidity of workholding. If I'm cutting a plastic, I'll have my Lead-in, Cutting and Ramp all at the same feed. Lead-Out can be same feed or greater. If I'm doing Stainless with small tooling, I'll set Lead-In and Ramp to half the cutting feed (in some cases)

3) In your Tool Library, you can renumber individual tools by double clicking on the tool and going to the Post Processor tab (last tab). There you can input any number you want. You can also do a global renumbering. You will have to click on the active file and then the icon that I circled

Re: Setting up Fusion for mill's limits and outputs.

Anonymous — Tue, 18 Apr 2017 16:58:20 GMT

Wow, thanks for the quick reply.

1. Yes, it is at the beginning and it does have limit switches. Is Machine coordinate origin (G28) setup when I locate the origin of the part/ material? I touched off the part for the location.

2. I am machining aluminum. Attached is an image from my feeds.

3. Thanks for the tool numbering... I hadn't setup my library yet.

Thanks again!

Re: Setting up Fusion for mill's limits and outputs.

LibertyMachine — Tue, 18 Apr 2017 17:02:19 GMT

I suppose a more accurate question for me to ask was: If you have limit switches, do they also act as Homing Switches, in that you reference the machine out against them upon start up?

Your Limit Switches and the G28: The G28 is a command for the machine to travel to it's "Home" position, according to the axis call-out. G28 X0 Y0 will home out the X and Y axis. If you aren't set up for that homing function, you would likely get an alarm. What you can do, for testing, is to remove these lines (in red) and see what happens to the code. Do these things though: Cut air well above the part, or have no part in the vise. Would hate to see something go really bad...

O1001 (DELETE)
(T1 D=0.5 CR=0.03 - ZMIN=-0.177 - BULLNOSE END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

lots of unimportant G-code here

N1155 M09
N1160 G28 G91 Z0.
N1165 G49
N1170 G28 X0. Y0.
N1175 M30

If that works well, we want to see if your machine will accept a G53 in place of the G28 (you will need to manually change for now) and you will also have to remove the G91. Your Line would look like this: G53 Z0. and G53 X0. Y0.

Re: Setting up Fusion for mill's limits and outputs.

Anonymous — Mon, 24 Apr 2017 15:18:56 GMT

Thank you for giving this advice for my issues. Through studying g-code and trials, I am understanding how this all goes together.... machining with gcode, that is. I work another business, and and don't use my computer all the time, but this advice is highly appreciated, and working with it now.

I will delete those and see how it goes. Per G28, or G53 for that matter, what is the z value for these positions? I have only been touching off the x, y values and then tool offsets... is that it?

Another issue I'm dealing with is the cutter offfsetting from the material in the y (+) direction, and cutting air for 1/8", instead of the part. Is this program or machine settings?

I may not respond right away, but I'm working with it... should have more time this week to get this all figured out.

Thank you much!

Re: Setting up Fusion for mill's limits and outputs.

Anonymous — Mon, 24 Apr 2017 15:47:41 GMT

And thanks LibertyMachine!