[gerraldpeters]

Hi All,

Did my first cut on my new FLA 100 a 2" x 2" x 0.75" MDF with a 1.5" circle in it. After cutting the circle looks like an octagon like. Any ideas what that can be?

Thanks so much.

Gerrald

[crane550]

Need more info. What's your CAM software and what are you using to control your machine?

[gerraldpeters]

Oops Sorry

I Use Mach 3 and CAM software is AlibreCAM. The full version.

Use a Gecko 540.

If there is anything else needed please let me know.

[crane550]

Can you post your G-code? Also in the Mach window preview, does it look like a circle or an octagon? also a picture of the cut would be helpful.

What I am going with this info is figuring out if we are looking at a software or hardware issue.

[LouF]

Have you adjusted your machine in Mach3 Motor Tuning?


Lou

[gerraldpeters]

@Lou,

I do have adjusted Mach 3 so that my movement is correct. So 1" forward is 1"

Here are the G-cade and a pic

[ger21]

Post a picture of the actual cuts.

[gerraldpeters]

Here is a pic of the cut.
Hope you can see what I mean.

[ger21]

The problem is with your CAM program . The g-code is exactly what you got. There are no arcs or circles in the g-code, only the straight segments you see. You'll need to learn how to get AlibreCAM to output arcs or circles.

[crane550]

I have not put your code thru Mach3 yet so I can't say for sure, but looking at your actual cut it looks more like a programming issue then a mechanical one. I will copy and paste your code into my own machine tomorrow and check and see if I can get the same results. Then we can narrow it down to your post processor or mach3. I think it's going to be in your post processing.

Here is circle I have generated similar to yours. The specs: 1.5 diameter, zero is the center on top of the material. Depth passes of .125". Can't remember the feedrate, but your machine will only cut as fast as mach allows. It assumed a 1/4" bit. 3/4" deep cut.

Take a practice air cut first, then try this one and show what you get. I ASSUME NO LIABILITY.

( circle )
( File created: Sunday, May 13, 2012 - 09:08 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 4.000, Y= 4.000, Z= 0.750)
()
(Toolpaths used in this file:)
(Profile 1)
(Tools used in this file: )
(1 = End Mill {0.25 inch})
N100G00G20G17G90G40G49G80
N110G70G91.1
N120T1M06
N130 (End Mill {0.25 inch})
N140G00G43Z0.8000H1
N150S12000M03
N160(Toolpath:- Profile 1)
N170()
N180G94
N190X0.0000Y0.0000F100.0
N200G00X0.0000Y0.6250Z0.2000
N210G1Z-0.1250F30.0
N220G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N230G3X0.0000Y-0.6250I0.6250J0.0000
N240G3X0.6250Y0.0000I0.0000J0.6250
N250G3X0.0000Y0.6250I-0.6250J0.0000
N260G1Z-0.2500F30.0
N270G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N280G3X0.0000Y-0.6250I0.6250J0.0000
N290G3X0.6250Y0.0000I0.0000J0.6250
N300G3X0.0000Y0.6250I-0.6250J0.0000
N310G1Z-0.3750F30.0
N320G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N330G3X0.0000Y-0.6250I0.6250J0.0000
N340G3X0.6250Y0.0000I0.0000J0.6250
N350G3X0.0000Y0.6250I-0.6250J0.0000
N360G1Z-0.5000F30.0
N370G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N380G3X0.0000Y-0.6250I0.6250J0.0000
N390G3X0.6250Y0.0000I0.0000J0.6250
N400G3X0.0000Y0.6250I-0.6250J0.0000
N410G1Z-0.6250F30.0
N420G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N430G3X0.0000Y-0.6250I0.6250J0.0000
N440G3X0.6250Y0.0000I0.0000J0.6250
N450G3X0.0000Y0.6250I-0.6250J0.0000
N460G1Z-0.7500F30.0
N470G3X-0.6250Y0.0000I0.0000J-0.6250F100.0
N480G3X0.0000Y-0.6250I0.6250J0.0000
N490G3X0.6250Y0.0000I0.0000J0.6250
N500G3X0.0000Y0.6250I-0.6250J0.0000
N510G00Z0.2000
N520G00Z0.8000
N530G00X0.0000Y0.0000
N540M09
N550M30
%

[gerraldpeters]

Thank you so much.

Will have to investigate what I did wrong in the CAM process.

Gerrald.

[crane550]

The problem is with your CAM program . The g-code is exactly what you got. There are no arcs or circles in the g-code, only the straight segments you see. You'll need to learn how to get AlibreCAM to output arcs or circles.

You posted this while I was typing up my response. My thoughts exactly. If your going to have this problem, then this is as good as it gets as it means nothing is wrong with your system.

Good work, team. Welcome to CNCZone!

[BanduraMaker]

AlibreCam is visual mill. Somewhere in the machine setup area is a check box "output arcs as line segments" which mecsoft checks by default. Find that box and un-check it. You can also un check the helix option as well. Keep the spiral box checked as Mach 3 doesn't do spirals (at least, not in the usual way).

[gerraldpeters]

Thank you guys.

Yes I hope it is a cam issue too. I will keep you all informed. Need to travel this week so no progress until the weekend.

[BanduraMaker]

Set Machining preferences.

[gerraldpeters]

Thank you. When back from my trip I will look for this. Sounds like the issue