Corner slowdown rules...do you use them for art, or just dimensional stuff?

[motoguy]

Tom made a comment over on the CandCNC message board. To paraphrase, "corner slowdowns are only needed for tables that can't handle the quick transitions". Meaning, a table that doesn't have good accel, or is mechanically not rigid. I'm curious...when do you use (or not use) corner slowdown rules? I have come to lump them together with THC on/off rules, but I'm beginning to see they are two separate things.

I cut one of the tattered flags a few weeks ago out of 18ga. Used my regular THC off/corner slowdown rules. The dross was incredible on the back, and it took a long time to cut. I later cut an 18ga 36" square sign with script text. I left the THC rules intact, but removed all corner slowdowns. It cut great, cut quick, and was MUCH easier to clean the dross.

I'm getting ready to cut a 6-sided firepit from 3/16" material. Each side has a moose and a tree cutout. Looking at all these intricate cuts, it's going to take forever with corner slowdowns, and/or dross buildup. I'm thinking of removing the corner speed rules, and just engaging/disengaging the THC instead.

It's my understanding that the corner slowdown rules are really about bevel. For circles, slowing down will let the arg dwell longer, which removes bevel. When do you guys use corner slowdown rules?

[acourtjester]

I had stopped using the Cut rules completely and with 14 Ga and thinner I have a switch on the arc OK signal to have it on all the time.

[tcaudle]

Corner slowdown is only needed if the corners are getting rounded or have flat sections on an arc or circle. The CV actions in MACH favor speed (velocity) over tracking (following the toolpath) . What you do when you lower feedrate is you pull back the amount of acceleration you need to make a corner, or turn , so CV lets it track closer. The trajectory planner in MACH3 is quite primitive but in 2006 is was all that was available at a reasonable price. It was originally derived from EMC (later EMC2 and later LIUXCNC but that's another story). The new trajectory planner in LINUXCNC has a setting for tracking that lets you define how far from the toolpath you will allow it to deviate and it automatically slows down the feedrate to let the tracking hold that accuracy.
So for a MACH3 based system you want to run it with as high an acceleration as it can muster (something in the 35 IPS/sec range) and just use the DTHC off rule or in the case of small holes or small objects you can use the " Min Cut Length for DTHC" to keep the DTHC from turning on for that cut. Group the small holes or cuts on a separate layer and slow the feedrate for the whole Operation so you don't have to use a bunch of rules.

[East German]

Hallo
I'll do the same in the drawing.
My layer Name is: hole ....inside small .....inside big...... ork
(Without radius compensation) and outside.
I load an old job file in Sheetcam and always get the same layer , another the new drawing and ready.
This works very well.

Regards Peter

[jimcolt]

The whole idea for slowing on holes is to allow the bottom of the plasma arc to "catch up" with the top of the arc.....at ideal, dross free cutting speeds when using air as the plasma gas...there will be a 5 to 15 degree (depending on material thickness and consumables and torch model) lag angle in the arc. When you slow down to the point that the arc is straight....expect higher heat input and dross (though low speed dross is easy to remove).

Think about cutting holes with the arc lag. A hole is essentially a constant left hand turn, and with the arc lagging expect that the bottom of the arc will tail back and create a smaller diameter on the bottom of the hole. Slowing down produces dross, but minimizes the lag and produces less taper in holes. Small diameter holes are worse as the "left turn" is sharper, larger diameters (usually diameters of larger than 1") can be cut acceptably without any slowdown.

On my machine I can set an automatic slowdown (to 60% of the program feed rate) on all holes under a certain diameter....I have the diameter set at 1" and it seems to work well. Here is a pic of holes on 1/4" steel with rough top and bottom dimensions using the 60% feedrate cut with Powermax using 45 amp shielded process, note that the variation between top and bottom diameters minimizes as the hole diameter gets larger

dimensions.jpg (106.35 KiB) Viewed 1646 times

dimensions.jpg (106.35 KiB) Viewed 1646 times

Slowdown rules are important for most fine features as well...think about the lag angle of the arc and what it can do on a sharp square corner (bottom washout)...a properly set slowdown will improve cut quality....too slow and you add heat and increase kerf width.

There are high end high definition class plasmas (Hypertherm HPRXD systems) that use super co-ordinated control of height, lead In shape, plasma /shield gas changes, plasma off timing and overburn distance.....with all of these parameters varying for each hole diameter, material thickness and amperage level. These systems use a large database of parameters based on lab research that are embedded in CAM software....the software recognizes holes in the CAD drawing and automatically modifies the cut profile as well as all parameters to create holes with zero taper. this process is called True Hole. Since it requires the ability to to have separate plasma and shield gasses and the ability to switch from one gas to another during the pierce / lead in on hole cutting.....it will not work with a typical air plasma system...unfortunately.

Jim Colt Hypertherm