Newbie with a few quality questions
-
oldmountaincrafts
- 2 Star Member
- Posts: 88
- Joined: Sat Oct 12, 2013 7:46 pm
Newbie with a few quality questions
We have a new 4x4 LDR water table and are having a blast testing everything out and cutting away. Being totally new to the plasma side of art, we have a few questions. I've downloaded and cut several files from this site and they look pretty great when they are finished. I'm a designer myself, but never for plasma cutting. I'm finding that some of my files look pretty awful when cut out and I'm at a loss as to where to start tweaking things. One of the first things I'm finding is that all my lettering is being rounded off. Even though the file looks fine and is very straight when using a serif font, once cut it is rounding every edge over? Is this a problem with the design part or how I generated the g-code? As I said, we are complete newbies to plasma cutting. We also have a laser for our business that I use the same files with and don't have any problems. That may be part of my downfall, but I'm just not sure. Any and all help is appreciated.
LDR Motionsystems 4x4 plasma
Hypertherm 45
Laser 4 X 4
Full woodshop
Hypertherm 45
Laser 4 X 4
Full woodshop
-
dhelfter
- 2.5 Star Member
- Posts: 125
- Joined: Wed Sep 09, 2009 11:18 pm
Re: Newbie with a few quality questions
What thickness material, amperage being used, and size of feature (letter size) all have an affect on rounded corners. The table is set with an acceleration of 35IPSs You can raise this, however we have noticed that going higher than 50 causes some vibration. There is a difference between acceleration and controlled acceleration.
The reason corners are getting rounded is because the the machine attempts to stay at a constant velocity. Think of a car, if you were driving on a curvy road and you tried to keep the car going 55mph you would need to "round" the corners, hard to take a 90 degree turn at 55mph. The quicker you can accelerate the better. This number comes from power available, and mass being moved.
Another albeit less contributing factor is the fact that plasma is an electrical arc process, so if you slow down the "tool" widens. You can not help but slow down on a corner, even million dollar machines have to, they can accelerate to insane numbers so it appears like they don't but they do!
One more contributing factor is number of nodes. Many drawings have features made up of hundreds or even thousands of nodes. This requires thousands of lines of code to be processed just to cut a simple shape. Take a circle for example. Many cad programs output a circle with lots of small lines, a true circle should only have 4 nodes.
There are several things you can do:
1. Cut at a lower amperage, which requires less speed therefore the machine will be at the "instructed" velocity a higher percentage of the path.
2. Cut out of thicker material, basically same reasoning as #1. You will be cutting slower
3. Enlarge the letters, this allows the machine to have "room" to accelerate and decelerate.
4. In mach3 turn cv off for an angle greater than "X" (you pick the angle)
5. In sheetcam use the rule editor to create a cutting rule that instructs the machine slow down on corners and turn dthc off (because we slowed down the voltage will increase so we want thc off).
Obviously 1 through 3 is a bandaid. If you need tiny letters out of thin material with the amperage you have available, your hands are tied!
Number 4 is fine, the problem is you have to remember when you do not want cv off you have to tell the computer. Also it will not turn thc off and you do run a risk of the torch touching the metal.
Number 5 is what I recommend. This is why I am a big fan of lots of layers. In sheetcam you can then use path rules for one layer and not the next. So you could have all small features on a layer and use your corner slow down rule, then on inside features that are larger you can not use it.
As stated before one other option is in mach3 motor tuning, increase acceleration. Our machine will accelerate much higher than what we set them at. 75% of our customers are cutting thicker more mechanical components. In these cases you are cutting slower, and less detail so 35 is fine. Feel free to increase the numbers, the one thing you MUST do is make sure the number for the Y and A axis are exactly they same, because they are slaved together. If you want to adjust acceleration I would create a file with just one letter (the one that cut the worse) and change acceleration, cut letter then tweak as needed till you are satisfied.
I would recommend using path rules in sheetcam though. You have much more control that way.
Feel free to call if you need help.
Thanks
Dan
LDR Motion Systems
The reason corners are getting rounded is because the the machine attempts to stay at a constant velocity. Think of a car, if you were driving on a curvy road and you tried to keep the car going 55mph you would need to "round" the corners, hard to take a 90 degree turn at 55mph. The quicker you can accelerate the better. This number comes from power available, and mass being moved.
Another albeit less contributing factor is the fact that plasma is an electrical arc process, so if you slow down the "tool" widens. You can not help but slow down on a corner, even million dollar machines have to, they can accelerate to insane numbers so it appears like they don't but they do!
One more contributing factor is number of nodes. Many drawings have features made up of hundreds or even thousands of nodes. This requires thousands of lines of code to be processed just to cut a simple shape. Take a circle for example. Many cad programs output a circle with lots of small lines, a true circle should only have 4 nodes.
There are several things you can do:
1. Cut at a lower amperage, which requires less speed therefore the machine will be at the "instructed" velocity a higher percentage of the path.
2. Cut out of thicker material, basically same reasoning as #1. You will be cutting slower
3. Enlarge the letters, this allows the machine to have "room" to accelerate and decelerate.
4. In mach3 turn cv off for an angle greater than "X" (you pick the angle)
5. In sheetcam use the rule editor to create a cutting rule that instructs the machine slow down on corners and turn dthc off (because we slowed down the voltage will increase so we want thc off).
Obviously 1 through 3 is a bandaid. If you need tiny letters out of thin material with the amperage you have available, your hands are tied!
Number 4 is fine, the problem is you have to remember when you do not want cv off you have to tell the computer. Also it will not turn thc off and you do run a risk of the torch touching the metal.
Number 5 is what I recommend. This is why I am a big fan of lots of layers. In sheetcam you can then use path rules for one layer and not the next. So you could have all small features on a layer and use your corner slow down rule, then on inside features that are larger you can not use it.
As stated before one other option is in mach3 motor tuning, increase acceleration. Our machine will accelerate much higher than what we set them at. 75% of our customers are cutting thicker more mechanical components. In these cases you are cutting slower, and less detail so 35 is fine. Feel free to increase the numbers, the one thing you MUST do is make sure the number for the Y and A axis are exactly they same, because they are slaved together. If you want to adjust acceleration I would create a file with just one letter (the one that cut the worse) and change acceleration, cut letter then tweak as needed till you are satisfied.
I would recommend using path rules in sheetcam though. You have much more control that way.
Feel free to call if you need help.
Thanks
Dan
LDR Motion Systems
-
Metriccar
- 3.5 Star Member
- Posts: 508
- Joined: Fri Apr 26, 2013 9:56 pm
Re: Newbie with a few quality questions
The kerf of the plasma cutter alone will make corners have a bit of rounding as well. Which is why you want to use the smallest and lowest amp nozzles that we still cut the metaL
-
urbnsr
- 3 Star Member
- Posts: 329
- Joined: Wed Dec 26, 2012 6:13 am
Re: Newbie with a few quality questions
If the rounding amount is small, and more noticeable on the back side, and you're using SheetCam, you can use SheetCam's Loop sharp corners (defined in the Operations window) to help with that. The thicker the material cutting, the more noticeable it can be. If the rounding is a large amount and somewhat consistent, you may have a trajectory issue with the controlling software's CV setting(s).
HTH
Paul
HTH
Paul
