PDA

View Full Version : Finished Set Up - First Test Part


mbellon
06-23-2013, 08:12 PM
I finished setting up my Stinger I with FTC and laser (with a few questions answered by Mick - THANKS!)

A) I milled my spoiler board flat.

I used VCarvePro (7) to set up a piece of material 0.010 inches thick with its Z set at
the top and the length and width of my work area. I used a 2.5" spoiler board tool.

B) I did a calibrate switch.

I put a 0.25" end mill in the router.
I put 3 pieces of computer paper on the spoiler board. That's about 0.012" thick in total.
I gently lowered the end mill onto the paper until I could barely move the paper.
See the picture below.
I did the calibrate switch.
I got a blue box next to Z in WinCNC.

Now my Z0 is slightly above the absolute Z0 of the spoiler board. Even if I do full
thickness material cut I will not cut through the piece into the spoiler board.

C) From now on I lay out my pieces with the Z0 on the bottom of the piece (layout). I
never use touch top or the Z0 assist device.

The software knows to emit the G code to start cutting at the correct height because
my material thickness is set in VCarvePro.

The material has at least 1 inch of material surrounding the part I'm cutting out so
that I have no chance of ever hitting a hold down.

D) I put my first test piece on the spoiler board and clamp it down.

E) I turn on my laser and line it up with the edges of the material.

F) I hit laser X0/Y0.

I get two green boxes, one for X and one for Y. Now the X0/Y0 from my layout lines
up with the temporary/relative zeros of the machine.

I use "G92" each time I start the machine (after initializing it) to clear the previous
temporary/relative zeros.

G) I load the G code and start the cut.

The router moves to the FTC pad and measures the part, starts the router and off it
goes.

H) Time passes... The part is done!

Check out the pictures. The part is a desk grommet. Yes, I used a piece of scrap plywood. I knew ahead of time that it won't look the best. That was OK since this was a test piece, one to ensure I understood everything properly. I have a nice piece of birch for the final result.

Notice that the part is cut all the way through and yet didn't once touch my spoiler board. That's due to the slight Z offset of the 3 pieces of paper. I land up with "onion skin" which is trivial to remove. I use a trim router to finish the part.

Charlie_L
06-23-2013, 09:29 PM
Mark,
Fun to read. Nice write-up. Could even tell you were excited from your words, proud too.

Relative to not hitting the clamps. Keep watching because sometimes when I least expect it the tool goes in a direction I hadn't planned. For me it is usually after done cutting and the post processor takes it back to x and y absolute zero. I'm going to modify the post processor so when it makes that traverse it is raised to the top of the z travel, absolute z=0. Otherwise, it scares me as it comes near the clamps.

Great success and thanks for the write-up.

Mick Martin
06-24-2013, 12:07 AM
Great job Mark, setting Z0 on top of the spoilboard is the way to go, plus you don't cut into the spoilboard. Johnnycnc told me a way to check my tap file to make sure it would not cut into the spoilboardand, open to tap file in note pad then press Ctrl + F (find) then type z- in the search and press enter. There are a few extra functions in Wincnc which are nice to know about the preview (eyeball icon) this shows a preview of your toolpath and the simulate function which can be found under the edit tab this will show any error in your tap file. You told me you had a machining background, I can see that in your write-up.
The first few cuts are nerve wracking, but after that it becomes easier ....... good job [clap]

Mick Martin
06-24-2013, 12:23 AM
charlie,
When I draw my material in Aspire I use the offset vector button and draw a square 1" smaller than my material, I then create my project within the inner box. I made my wooden clamp so they grip/hold on 1/4" material, I normally use 1/4" endmill to do my profile cut, so that leave me 1/2" clearance.

mbellon
06-24-2013, 12:47 AM
charlie,
When I draw my material in Aspire I use the offset vector button and draw a square 1" smaller than my material, I then create my project within the inner box. I made my wooden clamp so they grip/hold on 1/4" material, I normally use 1/4" endmill to do my profile cut, so that leave me 1/2" clearance.

I do the same thing as Mick. My hold downs are very low profile and only need a bit more than 0.25" for a good hold down.

mbellon
06-24-2013, 01:29 AM
Mark,
Fun to read. Nice write-up. Could even tell you were excited from your words, proud too.

Relative to not hitting the clamps. Keep watching because sometimes when I least expect it the tool goes in a direction I hadn't planned. For me it is usually after done cutting and the post processor takes it back to x and y absolute zero. I'm going to modify the post processor so when it makes that traverse it is raised to the top of the z travel, absolute z=0. Otherwise, it scares me as it comes near the clamps.

Great success and thanks for the write-up.

Thanks! I have a machining and CNC background and I hope my approach might be useful to some. I'm new to winCNC and CAMaster. I get the Hibbie-jibbies just like I get when learning a new machine or starting a new, complex part the requires a novel hold down.

One of the fundamental rules of CNC - which you point out - is always watch when the gantry is in motion.

In VCarvePro 7 one can set the safe height - above the material (and hold downs) - so as to be safe. None-the-less, if you find how to get an automatic move to max Z please let me know. I like the idea.

Mark Meyer
06-24-2013, 06:14 AM
Mark, with the care you have taken to avoid milling your spoilboard, one more thing you can do to prevent cutting into it is to go into the WinCNC.ini settings file and set your Z axis boundary to 0.00.

It's in the "soft limits" paragraph, and you're looking for a section that looks similar to this:

[Soft Limits]
lolim=x-2.5 y-.04 a-500000
hilim=x76.679 y147.00 z0 a500000
lobound=z-0.125
softlim=1

It's the "lobound=z" setting you can change to 0.00.