Center Marking/Dimpling for Drilling

[Ironken]

Some questions on centermarking/dimpling.

I'm running Sheetcam on my JD2 MAD 4x4 and would like to learn how to dimple for drilling.

My first question is how do I draw the dimple in CAD? Do I just make an extremely small circle or do I use the center mark feature in Draftsight? That feature makes a crosshair type entity to which I don't know how Sheetcam would interpret.

Next, how would I create the operation in Sheetcam amongst other profiles that would be cut (out of 5x3x.250 rec. tube)?

Thanks for any advice.

[tnbndr]

Do you have a scribe set up on your machine?
I draw a very small, 1/16" diameter circle and assign my scribe tool to it. I makes a very nice dimple for starting the drill.
If you are planning on plasma cutting the dimple or hole it may be hardened so you may have to use a carbide or cobalt drill bit.

[Ironken]

Thanks Dennis! I do not have a scriber on my machine. I do have cobalt drills though. I built a removable fixture in my water table to cut profiles in square and rectangle tube. It saves me a huge amount of time. To further save time, I wanted to include a dimpling operation while the part is in the machine to save time laying out a few holes that are too small to cut. I have templates and transfer punches but why not let the machine do the work if possible.

[steel 35]

Don't give up it works very well, as for the drawing all it takes is a small circle, I use 1/4" .
Sheetcam is adjusted in a drill operation that can be adjusted to the size you want.
Hard part is making a new tool for it.

[acourtjester]

I do it differently I use a scribe but draw out the pattern for the holes and use a circle diameter of 0.001" at each drill locations and use my Pen tool (plasma no cut commands). Attached is the SheetCam layout this was for location of mounting drill holes for linear bearing, hole size was 3/16" worked out great.

marking.JPG

[jimcolt]

On the Plasmacam tables (equipped with Advanced Motion Control) there is a drawing function called "point"....which is just that, a single node with no movement. In the software is a timer setting from xero seconds and up. The part file looks at this point as another cut path, but with no movement and it fires, then extinguished the torch for the exact time that is set by the operator. Usually the time I use is around .02 seconds, beautiful, round dimple, and because it happens so quickly there is not a problem with hardness (hardness created by an air plasma is a function of the 80% nitrogen in air combined with the heat from the molten metal, called "nitride hardening" or "nitriding". With the dimpling process this does not seem to occur. Jim Colt Hypertherm

[tcaudle]

SheetCAM knows the difference between a hole for drilling and center punching and a circle to cut. If you draw a circle in CAD then setup a "drill" tool in SheetCAM in the Plasma toolset it can peck pierce the cneter of the holes . Blowing full pierce holes does not yield a very clean or round hole to use if the position needs to be accurate. The plate marker method works the best. peck center marking (not a full penetration) with a torch is a standard part of the POSTs we provide with CandCNC for SheetCAM. If you have a Hypertherm with the RS485 serial port you can control the AMPS of the peck pierce too. A peck pierce is not really a pierce at all. Its just a mark in the metal that doe not completely penetrate so it does not burn out the sides and does not harden the steel.

[FazQuaz]

Watch this video: https://arclightcnc.com/marking-drill-s ... nch-plasma
I do it exactly like this video and it works PERFECT!

[Ironken]

Gentlemen, thank you for all of the help! I bookmarked this page and along with Arclight's video posted above. I am going to give it a go with the info you guys posted up and report back. Thanks again to all of you.

[acourtjester]

Thanks for posting I did a small test and things worked out very well I use a 45 amp nozzle on my Hypertherm PM65 set at 20 amps. As in the video I had to make the first dimple a separate layer and outside the useable area of the cut but all works as stated. I don't have the RS485 and I used a different post processor.

DSCN3223.JPG

[tcaudle]

This may help some with CandCNC controls and using a recent SheeCAM POST:

UsingPlasmaPeck.pdf

It has a POST setting (page 63) that tells it that a "Drill" tool is to be used as a peck device.

You just have to make sure the peck hole on your drawing (so it can find the center) is the same size as the drill tool you define in the toolset. I just make all my peck spot holes 1/4" and use a 1/4" drill size

The short cycle of the torch only works if purge air is on so on the first peck spot it first fires the torch in the air then goes down and does the peck. The rest of the pecks need to be within a second or two .

While it supports the RS485 and the Arc Current control it does not have to have that to work. The start height sets the arc gap on each one
For MACH you need the 11J or the 11N post. For CommandCNC you need the 24D or higher rev post,

If you want to revert back and use a real drill then you just cahnge the option in the POST Options. It also supports center punching with a plate marker using the same type process (drill tool) but it has to be named "CenterPunch" as tool name.

[steel 35]

Here is one I needed to adjust the hole size's to get them a little closer together; Using Toms method. As you can see a little bit of clean up for some of the first peck's that got splatted with the latter is needed because they are very close to each other.
Nice and round

drill.JPG

[motoguy]

Thanks for the info! I'll come back and re-visit this!