Two problems with first run

Post anything you want to discuss with others about the software.

Two problems with first run

Postby AndyRN » Sun Dec 30, 2018 1:56 am

1. I tried a generic circle and it was not a circle, more like an octagon. As the bit did its helical patern into the wood it was a perfect circle but once it got to depth and expanded out the circle it was not smooth at all.

2. When I would run the above posted circle program, Z would bottom out and not stop until it hit a limit switch. I'm not good with the different types of home; however, I did a machine home then I centered the spindle over the stock origin and zeroed out the xyz axis. after that I would 'cycle start' and z would go neg height until it hit the limit switch. In fusion I used the UCCNC post process; below is the first few lines of code. In order to get the porgram to work I would have to select the option to start from "G0 X-0.0926 Y0.2187" and then it would run fine from there. Not sure what code above that point is causing the problem or something I'm doing to cause the problem.


(T1 D=0.5 CR=0. - ZMIN=-0.6553 - dovetail mill)
G90
G0 G53 Z0.

(2D Adaptive3)
T1 M6 (dovetail mill D=0.5 1/2 bit Andy)
S5000 M3
G64
G54
M8
G43 H1
G0 X-0.0926 Y0.2187
AndyRN
 
Posts: 7
Joined: Sat Dec 22, 2018 2:16 am

Re: Two problems with first run

Postby Robertspark » Sun Dec 30, 2018 10:22 am

Please post your entire code, trying to work out what exactly you are trying to do from what you've posted is impossible.

Please can you also post your machine profile too please.

What motion controller are you using (UC100 / UC300 / UC400)?

What version of UCCNC are you using? (if in doubt go to the "HELP >> ABOUT" screen)

Try to take the time to learn to read the gcode it will save you a lot of issues later on or to at least understand what you're asking the machine to do, there is nothing apparent as to what your issue may be from the above code.
On line 3 you do send the machine to machine co-ordinates location Z0...... normally this is upwards..... it could however be anywhere youve defined in your profile..... is it upwards, is it upwards with an offset?

You've asked the machine to setup the tool length offset to that tool stored in TOOLTABLE #1 (G43 H1)

(T1 D=0.5 CR=0. - ZMIN=-0.6553 - dovetail mill) (TEXT, LINE IGNORED)
G90 (ABSOLUTE DISTANCE MODE)
G0 G53 Z0. (RAPID MOVE {G0} IN MACHINE CO-ORDINATES {G53} WITH Z AXIS TO "0")

(2D Adaptive3) (TEXT, LINE IGNORED)
T1 M6 (dovetail mill D=0.5 1/2 bit Andy) (TOOL #1 {T1}, TOOL CHANGE {M6})
S5000 M3 (SET SPINDLE SPEED TO {5000 rpm} TURN ON SPINDLE {M3})
G64 (SET MACHINE TO CONSTANT VELOCITY MODE)
G54 (WORK OFFSET G54 )
M8 (TURN FLOOD COOLANT ON)
G43 H1 (SET TOOL LENGTH OFFSET {G43} FROM TOOL #1 {H1})
G0 X-0.0926 Y0.2187 ({RAPID MOVE {G0} TO X {-0.0926} & Y {0.2187})

I know I' going to come across as arrogant, but what exactly is a "generic circle"?
Is it an arc move? (G02 / G03)
Is it a load of G01 linear motion moves?
What step size have you defined in your profile?
How big is the "generic circle" ?
As an exaggeration .... say you have a set size of 1/4" and you ask for a circle of size 1" it will look jagged because it will have 12 steps that create your circle....
Rob
Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
...working my way through the 1000+ ways things don't work to find the one that does
UC400eth, UC300eth, UCCNC v1.2108, Neuron Lite
UCCNC v1.2108 Macro Manual
Robertspark
 
Posts: 1208
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England

Re: Two problems with first run

Postby AndyRN » Sun Dec 30, 2018 12:27 pm

Sorry should have been more specific. Thanks for the help

Pictures are worth a thousand words.



https://photos.app.goo.gl/ebzyqEwgpgQJE6HT6

https://photos.app.goo.gl/FGd6YfEpZki4zQk5A

https://photos.app.goo.gl/MtzEKw4KdGYnyEbY9

https://photos.app.goo.gl/9ZKbRTCWLWTcvt4V9

https://photos.app.goo.gl/8DFvnj1WsPHRUc466

Image

Image

Image

Image


(Don't think images will post so I provided links as well)

Generic Circle- I designed a circular pocket about 5" in diameter and about 7/16" deep to be done in 3 passes. As the CNC would make the helical plunge cut to start the pocket it would be a perfect circle, once the helical plunge cut reached the final depth and it started to work out the final diameter the circle was almost a perfect multi faceted circle. see pic above.

I read that I may need to adjust the Constant Velocity setting from the stock setting, does this sound accurate?

G43-I see...I should never need G43 because when I do a tool change I would have to reset Z to the new tool height manually, am I understanding that correctly? How do I have fusion stop generating the G43 code or should I just manually delete it every time? I looked at the Post Processing file and that is way over my head to manipulate, I am definitely not a coder.


My Setup:
UCCNC version 1.0249 with Gerry's 2017 Screenset from thecncwoodworker.com
UC100
3 axis router 4'x6' bed with y being the 6' section
I have no offsets set
I have it set to the standard xyz configuration, nothing reversed, machine home is the front left of the machine as I am looking at it from the front.
If I remember correctly I have my stepperdriver set to 1/4 microsteps (800 microsteps per revolution)
My z axis is a screw drive at about 5000 steps per inch and xy are belt drive at about 500 steps/inch velocity


As far as Gcode I am mildly familiar with it, I have to keep a reference sheet handy, I looked up all the M and G codes after I had the problem but I could not figure it out which is why I posted the question.

Here is more of the code, It is several hundred lines long but here is much more of it.

(T1 D=0.5 CR=0. - ZMIN=-0.6553 - dovetail mill)
G90
G0 G53 Z0.

(2D Adaptive3)
T1 M6 (dovetail mill D=0.5 1/2 bit Andy)
S5000 M3
G64
G54
M8
G43 H1
G0 X-0.0926 Y0.2187
Z0.5906
Z0.1969
Z0.0984
G3 X-0.2187 Y-0.0926 Z0.0854 I0.0926 J-0.2187 F33.33
X0.0926 Y-0.2187 Z0.0724 I0.2187 J0.0926
X0.2187 Y0.0926 Z0.0593 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z0.0463 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z0.0333 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z0.0203 I0.2187 J0.0926
X0.2187 Y0.0926 Z0.0072 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z-0.0058 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z-0.0188 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z-0.0319 I0.2187 J0.0926
X0.2187 Y0.0926 Z-0.0449 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z-0.0579 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z-0.0709 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z-0.084 I0.2187 J0.0926
X0.2187 Y0.0926 Z-0.097 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z-0.11 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z-0.123 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z-0.1361 I0.2187 J0.0926
X0.2187 Y0.0926 Z-0.1491 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z-0.1621 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z-0.1752 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z-0.1882 I0.2187 J0.0926
X0.2187 Y0.0926 Z-0.2012 I-0.0926 J0.2187
X-0.0926 Y0.2187 Z-0.2142 I-0.2187 J-0.0926
X-0.2187 Y-0.0926 Z-0.2273 I0.0926 J-0.2187
X0.0926 Y-0.2187 Z-0.2403 I0.2187 J0.0926
X0.2375 Y0. Z-0.25 I-0.0926 J0.2187
X0. Y0.2375 I-0.2375 J0.
X-0.2375 Y0. I0. J-0.2375
X0. Y-0.2375 I0.2375 J0.
X0.2375 Y0. I0. J0.2375
G1 X0.2377 Y0.0132 F50
X0.2393 Y0.0263
X0.2518 Y0.0777
X0.2534 Y0.0812
X0.2565 Y0.0888
X0.2593 Y0.0975
X0.2616 Y0.1072
X0.2632 Y0.118
X0.264 Y0.1298
X0.2639 Y0.1425
X0.2626 Y0.1561
X0.2601 Y0.1704
X0.2562 Y0.1854
X0.2509 Y0.2009
X0.2439 Y0.2168
X0.2353 Y0.2328
X0.225 Y0.2488
X0.2128 Y0.2646
X0.1989 Y0.28
X0.1833 Y0.2948
X0.1659 Y0.3087
X0.1468 Y0.3216
X0.1262 Y0.3333
X0.1042 Y0.3435
X0.0808 Y0.3521
X0.0562 Y0.359
X0.0307 Y0.364
X0.0044 Y0.367
X-0.0225 Y0.3679
X-0.0498 Y0.3666
X-0.0773 Y0.3631
X-0.1047 Y0.3573
X-0.1318 Y0.3492
X-0.1584 Y0.3389
X-0.1843 Y0.3264
X-0.2094 Y0.3118
X-0.2333 Y0.295
X-0.2559 Y0.2764
X-0.2771 Y0.2558
X-0.2966 Y0.2335
X-0.3144 Y0.2097
X-0.3302 Y0.1844
X-0.344 Y0.1578
X-0.3556 Y0.1302
X-0.365 Y0.1016
X-0.3721 Y0.0723
X-0.3768 Y0.0425
X-0.3792 Y0.0124
X-0.3791 Y-0.0179
X-0.3765 Y-0.0481
X-0.3716 Y-0.078
X-0.3642 Y-0.1075
X-0.3545 Y-0.1363
X-0.3426 Y-0.1642
X-0.3284 Y-0.1912
X-0.312 Y-0.2169
X-0.2937 Y-0.2412
X-0.2735 Y-0.2639
X-0.2515 Y-0.285
X-0.2278 Y-0.3043
X-0.2027 Y-0.3216
X-0.1763 Y-0.3368
X-0.1487 Y-0.3499
X-0.1202 Y-0.3607
X-0.0909 Y-0.3692
X-0.061 Y-0.3753
X-0.0307 Y-0.379
X-0.0002 Y-0.3803
X0.0303 Y-0.379
X0.0606 Y-0.3754
X0.0906 Y-0.3693
X0.1199 Y-0.3609
X0.1485 Y-0.3501
X0.1761 Y-0.3371
Last edited by AndyRN on Sun Dec 30, 2018 12:37 pm, edited 2 times in total.
AndyRN
 
Posts: 7
Joined: Sat Dec 22, 2018 2:16 am

Re: Two problems with first run

Postby ger21 » Sun Dec 30, 2018 12:34 pm

1) This is due to your CV settings. If your g-code is in inches, start by multiplying all the CV settings by 25, as the defaults are for metric setups.

2) When using the 2017 Screenset, you should not have any G43's in your code, as they can change the Z zero position. G43 only works with fixed length tooling, as with an ATC.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1265
Joined: Sat Sep 03, 2016 2:17 am

Re: Two problems with first run

Postby AndyRN » Sun Dec 30, 2018 2:51 pm

Thanks for the help, I appreciate it. Do you know how I would have fusion not generate that G43 when I do post processing? Or is there a better post processing I should use for my setup?
AndyRN
 
Posts: 7
Joined: Sat Dec 22, 2018 2:16 am

Re: Two problems with first run

Postby ger21 » Sun Dec 30, 2018 5:56 pm

Try using this post. I only did a quick test, but it should be fine.
Attachments
uccnc_NoG43.zip
(9.32 KiB) Downloaded 24 times
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1265
Joined: Sat Sep 03, 2016 2:17 am

Re: Two problems with first run

Postby AndyRN » Tue Jan 01, 2019 3:58 pm

I found the issue. It was not the G43 although I did remove that code manually. Thanks for the file I will give it a try.

The code that is causing the problem is the G53 Z0. I figured it out and removed it at the beginning; however, it is also generating the code at the end of the program as well which I did not catch.

So the G53 sets it to machine coords, but what is odd is I do have the home position for the Z height set to the top limit switch, so why would it go negative Z height to get to 0? I'll have to look into it a little bit more, for now removing the G43 and G53 seem to have fixed the machine. I have not rerun my circle but I did make corrections to the CV settings and it seems to be running better. I also turned down the velocity and acceleration, which seems to have improved the cuts as well.

Overall I am very happy with the CNC I built, It's been a hell of a project and a lot of fun to build.
AndyRN
 
Posts: 7
Joined: Sat Dec 22, 2018 2:16 am

Re: Two problems with first run

Postby Robertspark » Tue Jan 01, 2019 5:42 pm

What do you have written in this box as highlighted in the screenshot?
Attachments
2019-01-01 17_40_44-Settings.png
Rob
Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
...working my way through the 1000+ ways things don't work to find the one that does
UC400eth, UC300eth, UCCNC v1.2108, Neuron Lite
UCCNC v1.2108 Macro Manual
Robertspark
 
Posts: 1208
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England

Re: Two problems with first run

Postby ger21 » Tue Jan 01, 2019 6:10 pm

but what is odd is I do have the home position for the Z height set to the top limit switch, so why would it go negative Z height to get to 0


As Robert referred to, the default Z Home position in UCCNC is set to 50, so when you home the machine, your Z Machine Coordinate is set to 50.
Sending it to Z zero will try to send it 50" down into the table.

You do have it set to 50 in the screenshot you posted earlier.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1265
Joined: Sat Sep 03, 2016 2:17 am

Re: Two problems with first run

Postby Robertspark » Tue Jan 01, 2019 7:22 pm

Sorry forgot it was the 2017 screenset + Gerry was helping you + you had posted screenshots earlier.... I'm answering multiple questions on multiple forums.... :roll:
Rob
Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
...working my way through the 1000+ ways things don't work to find the one that does
UC400eth, UC300eth, UCCNC v1.2108, Neuron Lite
UCCNC v1.2108 Macro Manual
Robertspark
 
Posts: 1208
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England


Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 6 guests