Arc radius error

This forum is for general discussion about Aspire

Arc radius error

Postby Crone Design » Wed Mar 06, 2019 9:41 pm

I keep getting this error message "Arc radius too small, calculation failed". This happens with very simple programs that don't really have any tight radiuses. My machine is a Laguna Smartshop 1. I am pretty new to CNC, and both Laguna and Vectric don't really have any answers for me. The simulations of these files in Aspire run fine, but then I get this error message when I load the program in the machine. I am using the correct post processor, I know that comes up when doing a search online for this error. Could it be just a simple setting that needs to be changed in the controller? Anyone encounter this before?
Crone Design
 
Posts: 3
Joined: Tue Mar 05, 2019 3:08 am
Model of CNC Machine: Laguna Smartshop 1

Re: Arc radius error

Postby TReischl » Wed Mar 06, 2019 10:33 pm

Post up a snippet of the cnc machine code that includes a radius command line. According to what I researched those lines should begin with G02, G03.

A bunch of us can read cnc code so maybe we can help you out.
"If you see a good fight, get in it." Dr. Vernon Jones
User avatar
TReischl
Vectric Wizard
 
Posts: 2928
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Arc radius error

Postby IslaWW » Thu Mar 07, 2019 1:10 am

Also post what controller you are running
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1271
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Arc radius error

Postby Crone Design » Thu Mar 07, 2019 4:34 am

Ok here are some random lines I picked starting with G03. Couldn't upload pics on here for some reason.

Line No 40 N390 G03 X4.1621 Y1.3327 R0.1250
Line No 42 N410 G03 Y2.9821 R0.1250
Line No 46 N450 G03 X4.0539 Y4.5689 R0.1250
Line No 48 N470 G03 X2.1855 Y4.5064 R01250

The controller is the hand held controller that comes with Laguna CNCs.


I've attempted 5 projects so far and have only been successful with two of them. The other 3 got the same error message. The ones I was successful with both were done with engraving liner bits. The others that didn't work were all with a 1/4" end mill... not sure if this info matters at all. Thanks for the help.
Crone Design
 
Posts: 3
Joined: Tue Mar 05, 2019 3:08 am
Model of CNC Machine: Laguna Smartshop 1

Re: Arc radius error

Postby IslaWW » Thu Mar 07, 2019 4:47 am

Sorry Man... I am no help on the pendant controllers. Laguna Tech support?
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1271
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Arc radius error

Postby TReischl » Thu Mar 07, 2019 2:05 pm

Thanks for posting those. They were helpful, sort of.

Here is the thing, we also need to see the line before and after a G02 or G03 move to really check your code. Also it is important that the lines you show us are lines that cause an error.

My instinct is that the code is correct. There is nothing wrong with the lines you posted. Those are what arc commands look like when using radius style programming for arcs.

Here is what I would do in your situation:

Give the Laguna folks a call. Email them your design file and let them know you are using a .25 end mill. They are a training facility for Vectric products so have them post your file, test run it on their machine and send you the cnc code for testing on your machine. That will tell you if it is something specific to your machine.

Without seeing more of the program I am suspecting that you may have set some cutter compensation numbers that result in the tool not being able to cut the radii. That is a pure guess, nothing more.
"If you see a good fight, get in it." Dr. Vernon Jones
User avatar
TReischl
Vectric Wizard
 
Posts: 2928
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Arc radius error

Postby Crone Design » Thu Mar 07, 2019 7:07 pm

Thanks for the help guys... this is my first time using this forum, and it's really great to get such quick responses. I may have it figured out. I have been dealing with Laguna for the last couple weeks, but apparently I was just working with the wrong person. Another tech support guy from Laguna contacted me this morning and informed me that I was in fact using the wrong post processor. The Smartshop 1 actually uses the Swift post processor. I won't know for sure until tonight, but it seems like this should do it.
Crone Design
 
Posts: 3
Joined: Tue Mar 05, 2019 3:08 am
Model of CNC Machine: Laguna Smartshop 1

Re: Arc radius error

Postby rig gap » Fri Mar 08, 2019 3:11 pm

I agree with Treishl...the codes you posted look correct, but without the lines of code before and after the G03 (counter-clockwise curve), we can't calculate whether it is or not...just for grins, try changing your settings so the decimal output is 3 places instead of 4, and lie to your machine...change your cutter size to .124 (.001 smaller) but still use the 1/4" tool...sometimes when the curve radius is the same as the tool radius, that "radius too small" error can occur...just a thought.
rig gap
 
Posts: 41
Joined: Fri Jan 03, 2014 1:00 am
Location: Charlotte, NC
Model of CNC Machine: Home built aluminum and steel 3 X 4 CNC

Re: Arc radius error

Postby rig gap » Mon Mar 11, 2019 8:50 pm

rig gap wrote:I agree with Treishl...the codes you posted look correct, but without the lines of code before and after the G03 (counter-clockwise curve), we can't calculate whether it is or not...just for grins, try changing your settings so the decimal output is 3 places instead of 4, and lie to your machine...change your cutter size to .124 (.001 smaller) but still use the 1/4" tool...sometimes when the curve radius is the same as the tool radius, that "radius too small" error can occur...just a thought.



Sorry for the error...try changing the cutter size in the data base to .249 dia. (Not .124)...I was looking at the arc radius and transposed...getting old is a pain. (Lol)
rig gap
 
Posts: 41
Joined: Fri Jan 03, 2014 1:00 am
Location: Charlotte, NC
Model of CNC Machine: Home built aluminum and steel 3 X 4 CNC

Re: Arc radius error

Postby ger21 » Tue Mar 12, 2019 1:42 am

Try using a metric post.
I've seen some of those machines that would auto detect metric and inches, but arcs would not always work in inches
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1497
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Arc radius error

Postby fredfow3 » Wed Mar 13, 2019 2:29 am

Did you get this sorted out with the Swift PP? I know it uses I,J for arcs so maybe that was your problem...

VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.3]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.3]

Fred
fredfow3
Vectric Apprentice
 
Posts: 55
Joined: Thu Aug 04, 2016 1:40 am
Location: Massachusetts
Model of CNC Machine: Laguna Swift 4x4, Shapeoko S3 XL


Return to Aspire - General

Who is online

Users browsing this forum: kilrabit, ohiolyons and 26 guests