getting sharp internal corners - HELP

[Sharkman82]

I'm at my wits ends on how to get clean internal corners on the shark. I'm cutting out simple squares representing windows on scaled model buildings. Attached photos show square "windows" and how they were cut on the CNC shark. The material is 3mm HIPS plastic with a carbide plastic dual flute cutter with an o/a diameter of 2mm. The bottom left hand corner is where the shark makes its first plunge and returns to and does its step down. It cuts right into the corner at this point, does a little micro pause and continues, but it cuts at least a 5-6mm radius on the rest of the 3 corners. I understand that give the diamter of the cutter 2mm will leave a 1mm radius like in the bottom right hand corner which is fine BUT I'M OVER trying to figure this out. I can choose the "on line" on my profile cut options in VCARVE but that mean I have to get all my elevations and off set all the lines so the cut ends up to scale. All I want is the shark to cut into the corner instead of a radius - HELP!

[Consultingwoodworker]

The picture did not come through, but there are a few ideas;

What feed rate are you using?
How well is the material being held? Could it be flexing under the cutting load?
Have you tried changing from climb cut to conventional?
Are the dimensions of your cut accurate and the only problem is the radius?

You might want to try cutting the windows inside the actual line, then a second cut to finish it off.

If we discuss this, we might find the answer.

Ralph

[Sharkman82]

Thanks for the reply again Ralph,

Photos now attached. The shark rips through the HIPS plastic with ease and I'm running @ 5mtrs/ minute cut and running the FRO in my control @ 100%. Each Z pass of the profile cut is 0.8mm step (cutter is 2mm dia.) The dimensions of the squares are spot on with the scale in VCARVE. The only way I've come close to reducing the default radius is if I put a radius on the corners of the square (half the diam of the cutter) and force the shark to follow it by selecting to cut "on line" of the vector. This is a lot of mucking around considering I have all the elevations of the houses cleanly exported from Archicad, then have to go around to all the corners and add radius's. Also if i choose to cut "on line", my "windows" are technically 50mm bigger (not critical but I'm picky with scale hahaha)
Even doing thisi, t is still slightly more radius the the initial start and return point of the square (as seen in the photos bottom left) when the Shark starts cutting each square. The frustrating thing is that I can see what I want on the bottom left corner but can't replicate it for the rest? Also, I have noticed that each time athe shark does a full dept pass and returns to the bottom left corner of a square, it pauses slightly. Maybe it's a case of me actually learning to write it in the G code, which I'll pass on and buy laser cutter

Cheers,

Clint

[fison]

Clint,

If you open the .TAP files with notepad you can examine the code directly. By doing this and using a G-Code Reference guide (http://linuxcnc.org/docs/html/gcode.html) you can see what the code is telling the Shark to do.

I've discovered the default path control mode set by VCarve is set to motion blending with a tolerance of .1 inches (the actual code for this is "G64 P.1"). This allows the Shark to cheat a little and maintain a smooth cutting path without jerking a lot. This can cause the corners to be a different radius than you intend.

When I need the cutter to go exactly where I want I change the entire G64 line to "G61" this is the code for exact path mode. You may need to slow down your FRO a little as it can cause the Shark to jerk quite a bit.

If someone knows a good way to change the precision within VCarve or Aspire I'd love to know how.

Good luck,

[jeb2cav]

Hi Clint,

Some ideas from searching the Vectric forum. I have some projects coming up where I want a similar outcome, so spent some time looking.

It seems like there is an opportunity to get "better corners" by finding the optimal feed rate that you use with the tool setting before you select calculate. Another poster was able to control the feed rate outside of the VCarve, and had found a knee in the curve where he wasn't losing squareness on outside corners. It may be worth some experimenting with both to see if this improves the outcome of the "other 3" corners from your pictures.

Another idea that made sense to me is to add a peck/drill pass for each of the corners. Of course you'd have to go in and add those points for each of the windows - but you could use the same end mill. Run the drill pass first, then run your window cut out. This would get you a radius corner (as you point out that's what you're expecting), and enable you to cheaply compensate for any other weakness.

Fison's point is really interesting and clearly works for him. If it works for you, you may not need the drill pass. Or, adding the drill pass may remove the need to fool with the tap file.

This would be a really interesting question to ask on the Vectric forum - where is the tolerance (G64/61 value) set. I can't find any reference to it in the manual or elsewhere on the Vectric forum. I suspect that may be set in the Shark compiler. It appears that Mach software actually gives you that kind of control in it's more comprehensive control panel, so the Mach compiler may not actually write this G64 or G61 to their tap/g-code file.

Perhaps Tim Owens can provide insight into this aspect.

Lastly, I saw a lot of lessons learned about use of CAD or CAD like data. Often times there are duplicate vectors, and/or vectors that are not closed - both of which can lead to corner outcomes that are not expected or desired. Slowing the FR, the FRO slider, and/or the G64/61 change would have no effect in these cases (bad vectors). You'd have to clean them up/fix them after importing into VCarve.

Look forward to hearing if either of these solved your problem.

[Consultingwoodworker]

5 meters per minute is approx. 180 inches per minute (please check my math) which is WAY too fast in my opinion. I'd be willing to bet that either the plastic is flexing away from the bit, the bit is flexing away from the plastic, or a bit of each.

That would explain why the start corner is ok since as the bit pauses there, the bit and or material flexes back to the original state. Even full sized steel framed CNCs cutting with 1/2 bits will flex a bit under cutting load.

I typically run at 60 inches per minute with 1/4" bits, and run slower with smaller diameter bits.

Try running the same program again with the FRO set to 50%. I'll bet that you see an improvement in the corners even if they are not perfect. You will need to figure out the optimal speed for that bit/material combination.

Ralph

[RhB_HJ]

The only way I've come close to reducing the default radius is if I put a radius on the corners of the square (half the diam of the cutter) and force the shark to follow it by selecting to cut "on line" of the vector. This is a lot of mucking around considering I have all the elevations of the houses cleanly exported from Archicad, then have to go around to all the corners and add radius's. Also if i choose to cut "on line", my "windows" are technically 50mm bigger (not critical but I'm picky with scale hahaha)

Hi Clint,

How about adding that radius to your original drawing? Perhaps make it a tad larger than the radius of the cutter, just in case the SW compares the cutter diameter with the minimum radius in the drawing.

BTW I have similar projects on the board, with one advantage, where possible I cut windows etc. on the laser. So far the corners are sharp and square.

[Buc]

This information may help with the sharper corners. http://www.cncci.com/resources/tips/g61.htm

I also agree faster feedrates cause corner rounding. I run most of my jobs at 80 IPM and the FRO at 80%, So I can run an actual 80 IPM if I desire. It seems to work for me.

[Sharkman82]

Thanks for the feedback everyone, its great for a newbie like me!. I have taken a few days off work and I will play tomorrow with everything suggested.