Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: shasebroock on July 26, 2017, 03:57:03 PM
-
Hi, I am new to the forum, but not new to my CNC. I have a Legacy Arty 18 x 36 that I have owned for about 6 years. The machine/software seems to work fine when making parts, but when I try to make signs the letter quality is not good and it seems the problem is in the entry and exit points of the letters for the most part.
I have done everything I know to do to make sure it is not mechanical on my machine. Everything is tight, travel is smooth and seems fine to me. The problems with the letters is very consistent so they are always the same so starting to wonder if it is a Mach 3 adjustment or problem. I have VCarve 7.5 that I use to design and generate the G Code for the machine. The previews always look great, but the end result does not match.
I have attached a couple of pictures to show the problem and would appreciate any help and ideas you have. The pictures show the problems with the letters. I believe the letter style is Times New Roman.
Thank you, Steve
-
Steve,
Check that you are actually using the same angle of V-Bit that you are specifying in VCarve.
Tweakie.
-
Tweakie
Thank you for your reply, I am using the same bit that I programmed in VCarve that generated the G Code. 60 degree V Carve bit from Magnate.
Any other ideas, I just cant figure this out.
Steve
-
What he means, is to check if your 60° bit is indeed 60°.
It's hard to tell from your pictures, but this is a common problem.
Watch this video.
https://www.youtube.com/watch?v=NugdOnwnnPY
-
Got it that makes sense, I have down loaded these V bit test files and will try it tomorrow. I will report back with results. Thank you!!! Steve
-
Well I made myself geometry test files for 45, 60 and 90 V Carve bits. Of course ran the my 60 degree bit with the 60 degree program. I would say the 60 degree section is the best, so it doesn't appear that the geometry of my bit is the problem.
I did notice a little bump on the top side of the triangle, but this little bump is in ALL of the test cuts 55 through 65.
Any ideas where to look next? This is surely frustrating.
Thank you, Steve
-
Probably a machine rigidity, or backlash issue? Make sure everything is tight.
-
Yes to my best ability, the machine is tight, but smooth in motion in all directions.
I have a ticket out with Legacy CNC Woodworking Machines, but so far they have no solution.
Back to a software issue of some sort? I am not very good with the software pieces!
Steve
-
It's highly unlikely to be a software issue.
Does the issue shop up in the preview in V Carve Pro? If not, it's not a software issue.
-
Nope, the previews looks good in the software.
The errors are consistent every time I run the program on the machine. If it were mechanical, wouldn't the error change. I guess that is why I was going down the software road. And it is not just this project, it happens anytime I V Carve letters.
Any other ideas? Oh and I have also tried different feed rates and it always comes out the same.
-
There are a lot of 'chatter' marks in your machining.
I think you need to thoroughly check the rigidity of your machine (all axes) because something is just not right there.
My first thing to look for would be backlash / slack in the Z axis ( thrust bearing, spindle motor, etc.)
Tweakie.
-
Tweakie.CNC,
Thank you I will go back and check the things you are recommending.
Steve
-
Ok, here are the things I did today. Again my machine in a Legacy CNC Woodworking Arty 18" x 36"
• Leveled the table to within .0013” over the X travel 36”
• Leveled the table to within .0021 over the y travel 18”
• Measured the machine travel against the actual travel for X,Y and Z
o X was out ???? Forgot to write it down
o Y was out .0529” short
o Z was out .0124”
Used the Program in Mach 3 Advanced Settings Axis Calibration to change Motor stepper values (used my 6” digital caliper clamped to bed”) to measure travel. Did this multiple times to get closest measures I could.
• X Used 6” travel on digital caliper and now within .0005
• Y Used 6” travel on digital caliper and now within .0005
• Z Used 5” travel on digital caliper and now within .0005
• Went over all the gears, rail teeth, motor gears to check for slop
o Adjusted Y rail teeth to tighten
o X was good
o Z - I found there is .0035” slop in the Screw and Nut that moves the router up and down for the Z travel
This is the only thing I could not adjust as I assume it is wear
What is the tolerance on this?
Do I need to replace these two parts (see pictures attached)
So after all of this, hours of course later I ran part of a program to V Carve the word David that is part of one of my projects I need to get done. I would say it IS better. Please look at the pictures, particularly the top and beginning of the D and the tops of the V and I. These points are still not good, better but not good enough.
Could my slop of .0035” in the Z travel in my screw and nut cause this? I am probably not using the right parts names, so I have also included pictures of this.
Making some progress but still not perfect.
Thanks, Steve Hasebroock
-
Hi Steve,
That machining certainly looks like a great improvement on your earlier example. I think you are heading in the right direction.
A Z axis backlash of 0.0035" is not bad but V-Carving can place a lot of loading on the cutter so the whole machine really does need to be rigid. Have you tried taking a second pass at the work (same settings) ?
Tweakie.
-
Hi Tweakie,
I agree making good progress. I wrote to the manufacturer on the Z axis backlash, eager to see what they say.
I have not tried a double cut. Will try that in the next couple of days. Today and tomorrow are real busy so may not get to the machine before Wednesday.
I have learned a lot about CNC fine tuning.
Will report back
Thank you, Steve
-
I have my problem fixed. Fortunately the Manufacturer Legacy CNC Machine called me and signed into my machine and could see pictures of the problems.
He walked me through procedures to adjust out backlash on my X and Y axis. This machine has Rack and Pinion X and Y.
On Z I have about .0035 backlash, but he didn't think that would be my problem. My Z is nut and screw type, don't know what the right terminology is for that.
He also had me flatten a board on x travel and then another board on y travel. We were both very happy with the tram results. Never perfect, but really good and also decided this was NOT my problem.
Last after this I had good improvement, but still some problems in the quality of letters. Then found that the one 60 degree bit I was using performed great when set at 65 degree and the other when set at 67 degrees. Interesting as I ran the program suggested by CNCNutz and I would say that test showed by bits close to 60 degrees. Interesting!
Thanks to everyone that had input and ideas.
Steve
-
Definitely mechanical. My take on it: if it looks good, it is good. If you don't like the way it looks, then take steps to fix it. If you are able, get new parts for your z axis and replace them. The other thing you could do is adjust down your velocity and acceleration. If these two settings are too high, they will exacerbate your machine slop. What are your speed and velocity settings?
-
A couple of things to consider:
1. Z backlash - look at the code and see how deep the V is going into the material.
Then calc what .004" difference would make in the radius of the cut. You have what
you have, so live with it or fix it.
2. Material - different material will machine different so don't expect perfect results
from an inferior material.
3. Spindle runout - yes you have some, just a matter of degree and depending on movement
adds some to the problem.
4. Setup and how you define the machining also affect the final results
V carve probably provides for the proper movements in the code and Mach will implement
the code properly. If you want to have near perfect lettering your machines system must be capable of producing it and setup properly. It's that simple.
RICH