4th axis - CNC machine not matching Aspire 9.0 preview

This forum is for general discussion about Aspire

4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sat Jun 09, 2018 6:56 pm

Hello.

I started a new wrapping job setup. I needed a 1.4" finished diameter (which is a 4.398" circumference). Aspire 9.0 calculated all of this correctly and I was successfully able to mill my square stock down to 1.4" round stock.

I then needed the CNC to mill some 0.5" wide, 3/8" deep rabbits around the ends of my wooden dowel. As you can see below, I set up two 'pocket' rectangles in Aspire equal to 0.5" wide and 5" around the circumference; my tool path set the pocket depth to 3/8" deep.

Setup.jpg

You can see here that my Aspire preview shows that the rabbits should go completely around my dowel as designed.

Rabbits.jpg

In reality, the two rabbit pockets were only milled between 0 degrees to approx 150 degrees. The tool path depth was correct at 3/8" deep.

Actual.jpg

My 'create round tool path' and the two 'pocketed rabbit' tool paths both used the 0.5" end mill, I saved both tool paths into a single output file for my CNC machine. Is there a conflict when combining "automatically generated" Gadget vectors and "manually generated" user vectors? Does anyone know why the actual dowel wasn't milled around the entire 360 degree axis like the Aspire simulations showed? Thank you.
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby Rcnewcomb » Sat Jun 09, 2018 7:05 pm

Can you post your Aspire file?
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3064
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sat Jun 09, 2018 7:34 pm

Sorry. It should be attached now...
1) Blank to Cylinder.crv3d
(46 KiB) Downloaded 43 times
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sat Jun 09, 2018 8:24 pm

Interesting. Even when I start a new project from scratch and only add the pockets for my rabbits, I still see the same incomplete rotation results. So I'm thinking this has nothing to do with mixing the Gadget vectors with other vectors. Also, I'm pretty sure that my stepper is not losing counts because my rounding tool path from before made it all the way around; additionally, I would think the angle would "wander" if I were losing counts, but the start and stop rotations are always consistent. Other thoughts on what could be limiting my 4th axis rotations during the pocket tool path?

Test Pocket.crv3d
(36 KiB) Downloaded 29 times
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sun Jun 10, 2018 12:01 am

This time I tried running my 0.5" end mill down a profile line instead of in a pocket... The line profile tool path was even worse. The CNC would only rotate the dowel 50 degrees instead of the full 360 degrees; it would start at -20 degrees (i.e. start at 340 degrees) and rotate the 4th axis chuck 50 degrees CCW and finish at the +29 degree position. The updated Aspire 9.0 file is attached.

Test Pocket & Profile.crv3d
(45.5 KiB) Downloaded 31 times
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby 4DThinker » Sun Jun 10, 2018 1:05 am

My guess is that your controller isn't programmed correctly for your 4th axis. Or the A axis stepper is losing steps. Loose belt or loose coupler? Does your controller software report that the A axis has turned 360 degrees when it hasn't?

Are you holding the blank in a chuck or between centers with a toothed live center? The teeth may have stripped in the end grain of the blank.

4D
4DThinker
Vectric Wizard
 
Posts: 1121
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sun Jun 10, 2018 3:00 am

4DThinker wrote:My guess is that your controller isn't programmed correctly for your 4th axis. Or the A axis stepper is losing steps. Loose belt or loose coupler? Does your controller software report that the A axis has turned 360 degrees when it hasn't?

Are you holding the blank in a chuck or between centers with a toothed live center? The teeth may have stripped in the end grain of the blank.

4D


Hello 4D,

My setup is configured properly for a 4th axis as my post processor already allowed me to successfully turn the square stock into round stock... If I chose the wrong post processor (as I've accidentally done from time to time in the past), then the CNC machine would still be using XYZ coordinates instead of using the YZA coordinates. Additionally, if my belt, gears, and stepper motor were mechanically slipping, then I wouldn't have been able to turn successfully the square stock into round stock.

I've got a 4-jaw chuck holding my wooden dowel securely in place, so I know that my wood stock isn't slipping.

When I mentioned above that my A-axis was only turning from 0 to 150 degrees, or from "-20" through 0 to +29 degrees (a "50-ish" degree movement), I was reading those values from my controller. So no, my controller did not think it was making full revolutions when it truly wasn't.

In reflection, my 4th axis seems to work every time I've created "automatically generated vectors" using one of the many wrapping Gadgets... But this is the first time I've tried to "rotate" vectors by using a "manual" design. Has anyone else used Aspire 9.0 to successfully wrap "manually created vectors" around a 4th axis? Or does everyone exclusively use the wrapping Gadgets to create your wrapped designs?
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby IslaWW » Sun Jun 10, 2018 3:38 am

SCW...
Does the code in your cut file match the degrees (-20 to +29) that you saw on the controller?

As far as your last question goes, in all honesty, with the exception of preparing lessons for various rotary classes or presentations, I have NEVER used the gadgets. They are simply providing a simpler (to some) method of generating basic math.


Here is an example (a bit gaudy)

Rotary Plaid.JPG
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1109
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby Rcnewcomb » Sun Jun 10, 2018 7:12 am

What post processor are you using?
Can you ZIP and upload the saved toolpath files?

I noticed a few odd things:
On the pocket toolpath your 1/2" tool is set with a 90% stepover and a pass depth of 0.05", and your pocket is 0.5" which is the same as your bit diameter. The cut depth is 0.35" rather than 0.375". This type of cut is better done with a profile ON the line rather than a pocket. Also, I'd recommend you change the stepover to 40%, otherwise you may have issues on irregular shapes. Also, the pass depth of 0.05" is really shallow. You could probably change that to 0.25" on a 0.5" bit.

On the profile toolpath the cut dept is correct at 0.375". Even though the tool is set up to do a pass depth of 0.1" it looks like you've changed this in the "Edit Passes" section so it is still taking 7 passes. I saved this using several post processors and I do see the correct degree turns for what you have specified.

Note how it goes from A20.4628 to A-388.7928 just as you specified in your drawing.

Code: Select all
( X= 4.398, Z= 0.700)
( Diameter = 1.4000 Inches)
( X Values are wrapped around the Y axis )
( X Values are output as A )
()
(Toolpaths used in this file:)
(Test Profile)
(Tools used in this file: )
(1 = End Mill {1/2"} Up-Shear)
N130 G00G20G17G90G40G49G80
N140 G70G91.1
N150 T1M06
N160 (Tool: End Mill {1/2"} Up-Shear)
N170 G00G43Z1.7000H1
N180 S20000M03
N190(Toolpath:- Test Profile)
N200()
N210 G94
N220 Y0.0000 A0.0000 Z1.7000 F90.0
N230 G00 A20.4628 Y0.2500 Z1.4500
N240 G00 A20.4628 Y0.2500 Z0.9000
N250 G1 A20.4628 Y0.2500 Z0.6464 F60.0
N260 G1 A-388.7928 Y0.2500 Z0.6464 F90.0
N270 G00 A-388.7928 Y0.2500 Z1.4500
N280 G00 A20.4628 Y0.2500 Z1.4500
N290 G00 A20.4628 Y0.2500 Z0.9000
N300 G1 A20.4628 Y0.2500 Z0.5929 F60.0
N310 G1 A-388.7928 Y0.2500 Z0.5929 F90.0
N320 G00 A-388.7928 Y0.2500 Z1.4500
N330 G00 A20.4628 Y0.2500 Z1.4500
N340 G00 A20.4628 Y0.2500 Z0.9000
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3064
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sun Jun 10, 2018 6:42 pm

Rcnewcomb wrote:What post processor are you using?
Can you ZIP and upload the saved toolpath files?

I am using the following post processor obtained directly from the CNC machine manufacturer: 'Axiom_HHC_CNC_4TH.PP'

Here are my various toolpaths which include a pocket cut and a profile cut.
Spindle.zip
(3.08 KiB) Downloaded 29 times

Rcnewcomb wrote:I noticed a few odd things:
On the pocket toolpath your 1/2" tool is set with a 90% stepover and a pass depth of 0.05", and your pocket is 0.5" which is the same as your bit diameter. The cut depth is 0.35" rather than 0.375". This type of cut is better done with a profile ON the line rather than a pocket. Also, I'd recommend you change the stepover to 40%, otherwise you may have issues on irregular shapes. Also, the pass depth of 0.05" is really shallow. You could probably change that to 0.25" on a 0.5" bit.

Normally I use my 0.5" end mill to hog out material and so that's why I set the stepover to 90%. But as you imply, i did have to set the stepover to 20% to obtain good results when milling the square stock down to round stock. But for this case, I left the stepover at 90% for these rabbits because I expected them to be milled in a single, straight path (if that makes sense). So I do adjust the stepover value depending on the project.

I have had success before on flat "XYZ" projects when using pockets that are the exact width of the tool, so I thought I would chance my luck here too. But even when I tried cutting on the line of a profile line, I had similar results.

Correct, I'm being very conservative and going pretty light on the pass depth because my tailstock will move around if I'm too aggressive on my speed/feed... My tail stock is currently only clamped down; it's not yet bolted down (long story on why).

Great attention to detail! Yes, my cut depth is actually supposed to be set to 0.35" (the one file where the cut depth was set to 0.375 was actually an error that would have removed too much material). When I do the math, I will end up with a final mortise diameter of: 1.4" - (2 x .35") = 0.7". This will leave a buffer for glue and spindle alignment when I insert these spindles into the 0.75" tenon holes that I milled into some shelves.
Kitchen.jpg

Rcnewcomb wrote:On the profile toolpath the cut dept is correct at 0.375". Even though the tool is set up to do a pass depth of 0.1" it looks like you've changed this in the "Edit Passes" section so it is still taking 7 passes. I saved this using several post processors and I do see the correct degree turns for what you have specified.

Yes, for the reason mentioned above, I chose to overide the cut depth for fear of my endstock shifting.

Lol, it actually never dawned on me to look into the .mmg toolpath file to see what was going on (i'm still new to all of this). So, thank you for helping me to discover that Aspire is limiting the rotations, and that I'm not having a hardware issue. With that being learned, I might just edit the toolpath file to make the 360 degree rotations until I can figure out why Aspire is miscalculating the angles in the toolpath but not when calculating the simulations.

Sorry for the long post.
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby Rcnewcomb » Sun Jun 10, 2018 8:02 pm

So, thank you for helping me to discover that Aspire is limiting the rotations, and that I'm not having a hardware issue.

Actually, in the post processors I looked at it was NOT limiting rotations, it was moving more than 360 degrees just as you specified.

Here is some detail from the Test Profile mmg file that you provided
Code: Select all
N220G00Z36.830
N230G00A-20.463
N240G00Z22.860
N250G1Z10.976F1524.0
N260G1A2025.815F2286.0
N270G00Z36.830


The other G code experts can correct me if I misstate something. As I read this:
N220G00Z36.830 does a rapid move of the Z to 36.83 mm
N230G00A-20.463 does a rapid move of the A axis to -20.463 degrees.
N240G00Z22.860 does a rapid move of the Z down to 22.86mm
N250G1Z10.976F1524.0 moves the Z to 10.976 mm
N260G1A2025.815F2286.0 rotates the A axis to 2025.815 degrees which strikes me as odd
N270G00Z36.830 does a rapid move of the Z back up to 36.830 mm

I'm curious about the A2025.815 command. I'd recommend contacting support@vectric.com as well as the company that supplied the post-processor file.
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3064
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Sat Jun 16, 2018 9:44 pm

Here's what I'm seeing on my 4th axis:
    Controller C+ turns my chuck "CCW"
    Controller C- turns my chuck "CW"

I'll have my CNC machine zeroed out and then start my program:
    "A-27.000" command rotates my chuck in the CCW (+ direction) by 27* to position 27.000*.
    "A387.000" command then rotates my chuck in the CW (- direction) by 54* to position 333.000*.
    this 4th axis rotation pattern repeats until I reach my desired depth.

It almost looks like my +/- direction is reversed either in the tool path file or in my CNC controller... I'll have to see if there's an easy way to switch the C axis direction in my 4th axis post processor file (seeing as how my +/- directions are correct when I run XYZ programs using the XYZ post processor file). Thoughts in general?


Read more: http://axiomprecision.proboards.com/thr ... z5Ich54sS7
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby mikeacg » Sun Jun 17, 2018 2:36 pm

If you want a 1/2" rabbet and you are using a 1/2" bit, why pocket it? Why not use a profile cut set to depth?
User avatar
mikeacg
Vectric Wizard
 
Posts: 642
Joined: Sun Nov 02, 2008 10:53 pm
Location: Newberry, MI
Model of CNC Machine: Camaster Stinger, Sidewinder, SB 4x4

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby SCW » Fri Jun 22, 2018 11:26 pm

mikeacg wrote:If you want a 1/2" rabbet and you are using a 1/2" bit, why pocket it? Why not use a profile cut set to depth?


As discussed earlier in this thread, I've tried both pockets and profiles on this rotating project and neither method is working for me.

However, I've pocketed to the exact width of an end mill many times before on flat projects and have NEVER had any unexpected problems. The Aspire simulations seem pretty good at letting you know if a bit will fit into the vectors or not. Which allows me to make tweaks and perfect the design before I even start to make sawdust.

FYI, I sometimes pocket things because I want to reference/measure other vectors from the edge of the pocket and not from the center of a pocket (which would happen if I used a profile line).
SCW
 
Posts: 26
Joined: Fri May 11, 2018 4:44 am
Location: Stillwater, MN
Model of CNC Machine: Axoim AR8 Pro+ (w/ 4th axis); Aspire 9.0

Re: 4th axis - CNC machine not matching Aspire 9.0 preview

Postby TReischl » Sat Jun 23, 2018 12:34 am

Earlier you asked for "thoughts" on this issue.

My thoughts are that you either have a machine or a post problem. Both of which were created by the machine company.

That said, if Aspire was the problem you would not be the only one bringing it up. That is an important concept. The software is used all over the world on a daily basis with all sorts of machines.

If'n I were you I would be zeroing in on the machine folks.

Edit: Forgot to mention. . . I set up your situation on my software/machine. No problemo. What I did note was that ALL my rotary moves were negative values. I am thinking you have post problems.

BTW, how do other rotary programs run on your machine? Or is this the first thing you have attempted?
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2078
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Next

Return to Aspire - General

Who is online

Users browsing this forum: No registered users and 18 guests