How to fix rounded inside corners

[djreiswig]

Cutting some 28ga steel for a friend. Having trouble with the inside corners
rounding. The ones with the long edge cut first seem to be good. The ones
with the short edge cut first are rounded. First time I've ever cut anything
this thin.
Bulltear 4x8 with Bladerunner Ethercut
PowerMax 65 set to 40 amps with fine cut tip
I have the stop CV set to 89. Tried 60 with no change.

The tool is programmed to 325in/min per the book

I think it has something to do with the acceleration. I believe the X & Y are
set to 35 in Mach & the Z is 15.

[motoguy]

Try a smaller angle on your CV stop. Something like 45 degrees. X and Y accel set to 35 should be fine, though you can probably bump those to 40 if you'd like. I'm at 35 on my 6' gantry, and Matt said the 4' gantries can be a little higher. This whole CV / divot business is one reason I want to update to CommandCNC.

[djreiswig]

How does the CV work? The angle is like 105 degrees. How would making the number smaller make it cut better, and why does it work on the same angle when traveling the opposite direction (the one on the right)? I was thinking I needed to go bigger so make it stop on larger angles. Must not be the case.
I think we tried 45 and it made the good angles look worse.

[motoguy]

I've had to play with the CV, and set the angle in a way that didn't make sense in order for it to give the results I wanted. You can try bumping your acceleration a bit, and see if that helps. The issue is a CV issue, though.

Perhaps you could change the line tolerance setting, to force it to stay closer to your line. Hose clamp an ink pen to your torch (clicky kind, with a spring loaded tip), put some paper on your table, use the plain "Mach 3" post processor, create an "ink pen" rotary tool, choose "contour" instead of "plasma", and draw the file on paper. Play with your settings this way, until you get the shape you want.

Then switch back to your plasma post processor, plasma tool, and cut. Way easier /cheaper than experimenting on metal.

As far as the differences in sides, I speculate it is do with the lines leading to the corner. The faster the axis is zooming towards a corner, and the faster it will be moving after the corner, the further away CV is going to start rounding the corner.

https://www.google.com/url?sa=t&source= ... xrpIXsIjlw

[djreiswig]

Interesting read. I'm not sure I totally understand it, but I'll just have to play around a little with the settings and see what happens. Thanks for the advice.

[jimcolt]

In simple terms, machines that can stay on the intended path at the required plasma cut speeds....and do this with high acceleration and de-acceleration rates will produce better corners. Keep in mind that as you de-accelerate into a corner that the plasma arc continues to melt and blow away molten metal at the same rate and at a fixed energy density. When the cut speed slows, the cut kerf gets wider (the plasma arc stretches out to maintain electrical connection with the metal), and worse, if the machine dwells in a corner.....expect a rather noticeable divot.

Corner divots are often caused by loose machines with some backlash in the drives (flex in motor mounds, loose pinion gears, etc.), but can also be caused by delays in the motion control software or electronics. In my experience (almost 40 years working with NC and CNC plasma) with tuning for maximum acceleration you will see ripples and pronounced lag lines when entering and exiting corners....this means acceleration is set too high for the mechanical design of the machine. High acc / dec will cause the machine to flex or cause the motors to exceed their torque / rpm capability causing these anomalies in the cut edge. Reduce the acceleration or gain settings and the entrance/exit ripples will minimize.

Better design of machines (zero backlash or flex, inertia matched, properly sized drive motors) and good machine control software will improve these issues. There are some great entry level cnc tables out there....and there are some that are not so great! Small motors on heavy machines are often a bad sign, and often it goes along with lower price.

Jim Colt Hypertherm

[BTA Plasma]

That problem your seeing may be in the way your drawing carries over to sheetcam. Make sure the radius is not carrying over. We recently had this issue with Designtofab cutting production duct work with a HVAC company where the D2F would output the last inside corner as a radius instead of a square corner. What does the display look like in sheetcam? That is a good place to start.

[djreiswig]

I'm pretty sure it was an actual corner. Some of the parts have 4 of these corner notches. Two cut good. The other 2 (diagonal from each other) cut rounded. I guess if it is a radius, that should show up as an I,J move in the gcode, right? I'll try and attach the drawing if anybody wants to play with it.

[djreiswig]

I changed the CV to 45 and did some dry runs tonight and it seems to be stopping on those corners now.
How low can I go on the CV without causing other problems? What will happen if I sent the angle even lower?
I thought I remembered Bulltear saying to set CV to 89 to get square corners. Will a lower number mess with my outside corners?

[BTA Plasma]

If you set it at 1 it will just do the same thing as exact stop on every geometric trajectory change.

[tcaudle]

The problem with doing CV tuning is its global for everything you cut and it handles some shapes better than others. One setting is not optimal for all cuts. One of the compelling arguments for LINUXCNC is its better trajectory planner and CV method. Unlike the old one that MACH is based on, it does not give preference to speed over accuracy (toolpath tracking) . It instead adjusts the velocity and acceleration to hold the tolerance set for the cut. The downside of that in plasma cutting is t messes with the cut dynamics (slower feedrates cause the voltage to increase and that results in torch dive). To combat that you have to have a system with a real time link between the volts and the actual feedrate. By doing that you can dynamically enable/disable the THC (lock Z moves) for short and frequent toolpath anomalies.

In a road race with lots of curves and turns the driver has two things to accomplish: get the fastest elapsed time, but don't run off the road by cutting corners and straying off the course. The drivers job is to adjust his speed to run up to the limits of the vehicles capabilities and stay on course The better the performance of the vehicle the better the overall speeds will be but you still need to keep it in the road!

[Bigdogbro1]

Make sure if you are using Inkscape that you don't have the little tiny node diamonds at the nodes as those indicate multiple nodes at the same location. Multiple stacked nodes can cause weird things to happen. Check you Sheetcam node locations as well at those corners.

[djreiswig]

We are using TurboCad and Draftsight, but good idea.
I played around with my acceleration and speed. X and Y are set at 600. It looks like I start to lose steps somewhere around 800-900. (My X and A were getting out of sync a little bit when I did a reference. I had the acceleration up to 50 and it really gets to going. Neither one of those adjustments seemed to make any difference on the corners, so I put them back.

[Bigrhamr]

When I open your drawing I get an open profile, the angle line in the lower right corner notch is missing. Don't know if that could be related to your issue or not. The rest of the drawing is clean, one node at each direction change.

[djreiswig]

I just downloaded it and looked at it, and it's there for me. Sheetcam didn't give me any open path errors, so I think it is okay.
We cut some more stuff tonight with the CV set at 40 and it was making good corners. Guess that must have been it. Thanks everybody for the help.