Vcarve Inlays not Locking?

This forum is for general discussion regarding VCarve Pro
jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Okay, thank... I will try that calibration method.

How to I adjust for calibration though? With the machine or within Mach3?

The initial test, most looks okay except for the circle. The diameter was 2.25" and it is 2.12" so there is a bit of something off there. Any ideas what would cause the circle to be off that much or what to do to fix it?

TIA

JoeM
Vectric Craftsman
Posts: 286
Joined: Fri May 29, 2015 1:51 am
Model of CNC Machine: Shop-Made Router
Location: Arizona

Re: Vcarve Inlays not Locking?

Post by JoeM »

jackson74 wrote: The diameter was 2.25" and it is 2.12" so there is a bit of something off there. Any ideas what would cause the circle to be off that much or what to do to fix it?

TIA
1/8th = .125. Maybe you told the computer you're using a 1/4" bit, but you actually used a 5/8" bit. Or maybe when you were creating tools in your v-carve database you copied an existing one, gave it a new name, but forgot to change the diameter.

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

1/8th = .125. Maybe you told the computer you're using a 1/4" bit, but you actually used a 5/8" bit.
I don't think so , the bits were correct. at .125" and pocket toolpath. I assume the pocket I created the bit runs "inside and left" as there is no settings. Since there are two vectors, the outside diamond and the inside circle that the bit would not cross that "circle" line and keep the circle vector diameter in tack at .25" as I set?

Seems weird that the circle diameter went from 2.25 to 2.12 roughly. The bit size seems logical but I know I used the correct bit and setting on it and I assume it has to run inside the vectors for a pocket toolpath.

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: Vcarve Inlays not Locking?

Post by glenninvb »

jackson74 wrote:Okay, thank... I will try that calibration method.

How to I adjust for calibration though? With the machine or within Mach3?

The initial test, most looks okay except for the circle. The diameter was 2.25" and it is 2.12" so there is a bit of something off there. Any ideas what would cause the circle to be off that much or what to do to fix it?

TIA
Did not read entire post but you adjust in Mach3... if travel is correct in all axis you need to look at machine deflection or other cause


jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Okay, so after more work I got the best inlay (since the problem started).

It had minimal chip out spots and looked about 90% perfect, still a few small spots. I did a complete clean and dry lube of the machine.

I did a recheck on a pocket circle and it was to be 1.75" diameter but is coming in at 1.735.

Any tips on how to get this a little better? Do I need to do that in Mach3? If so I have no clue how to do it...

TIA

glenninvb
Vectric Wizard
Posts: 1129
Joined: Thu Jul 18, 2013 4:58 pm
Model of CNC Machine: homebuild / VCP 8.0

Re: Vcarve Inlays not Locking?

Post by glenninvb »

jackson74 wrote:Okay, so after more work I got the best inlay (since the problem started).

It had minimal chip out spots and looked about 90% perfect, still a few small spots. I did a complete clean and dry lube of the machine.

I did a recheck on a pocket circle and it was to be 1.75" diameter but is coming in at 1.735.

Any tips on how to get this a little better? Do I need to do that in Mach3? If so I have no clue how to do it...

TIA
I posted two links in reply above that shows the process.... the second video (below) is more detailed

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Ahh, yes, My bad I forgot you posted the videos. Bad few weeks for me and just got back on the machine to try and fix these problems. I will watch and try some tweaks and report back.

Thanks!

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Can anyone recommend a dial indicator or such tool for doing the calibration? Not sure what to get or what the standard is for general woodworking on a desktop 3 axis cnc mill.

Thanks for any help!

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Okay, so I tweaked and calibrated the machine with a dial indiactor therough Mach3 (thanks for the video links). Pretty quick and easy , a nice feature. My machine was not off to bad but a bit on each axis.

I did another test inlay and it was for sure the best so far. Very close to perfect but still some chip out along the edges of the detail. The larger dog profile is 100% perfect.

Could the chip out around the edges be a speeds and feeds issue? I used a new Whiteside bit.

TIA

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

I cannot find a through search a solid answer as to what a good starting points for Feeds and Speeds for a .25 60 Degree V Bit for Vcarve inlays would be.

Any advice on what people are using for finer detailed work in hardwoods would be appreciated.

TIA

ElevationCreations
Vectric Craftsman
Posts: 130
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Vcarve Inlays not Locking?

Post by ElevationCreations »

I typically slow my feed rate down to 60ipm on my machine for inlays to get a decent finish on the V-Bit, my speed depends on the wood species I am working with.

jackson74
Vectric Apprentice
Posts: 58
Joined: Sun Oct 18, 2015 6:46 pm
Model of CNC Machine: Romaxx WD-1

Re: Vcarve Inlays not Locking?

Post by jackson74 »

Thanks... What RPM's are you running at 60ipm?

Peter Stenabaugh
Vectric Craftsman
Posts: 189
Joined: Wed Jun 07, 2006 7:26 pm
Location: Calgary, Alberta Canada

Re: Vcarve Inlays not Locking?

Post by Peter Stenabaugh »

Jackson, I havent read all your posts, however if you are cutting circles and squares etc to try to calibrate your machine you are totally wasting your time. I am a machinist and I have built a few cnc machines - all running Mach 3. Assuming that you know the process of using Mach 3 to calibrate your machine, here is what you need.

You need a dial indicator (a cheap one will do if it works properly). The dial indicator must have a magnetic base, or a magnetic back to allow you to position it - RIGIDLY' close to the axis you want to test. I use one with a 2" travel, just for safety but a 1" travel will work. These dials usually come with a 2" diameter face.

There are a couple of way to tackle this job depending on your machine and your equipment. Since your machine seems to be 'close' to calibrated this will be REALLY easy. Assuming now that you have set up your dial indicator, make sure that you jog the X axis in the direction towards the dial indicator, just a wee bit to ensure there is no backlash in the system.

Set the dial indicator so that the tip just touches the machine and moves the needle about 0.010" - that way you know it is in contact with a bit of pressure. Make sure it set up square to the machine and not on an angle. Rotate the outer rim of the dial indicator to Zero the scale. Now using Mach 3 calibration, tell the machine to move 0.900" towards the dial indicator. the machine should move in that direction and your dial indicator should turn 9 times and the needle should be EXACTLY on Zero.

If your dial indicator is on Zero you are good, so then you need to tell Mach 3 how far the machine moved, so input .900" and press enter....... theoretically that axis is calibrated. Repeat the process for the other 2 axiis.

Ok, better then that..... the farther you move the machine the more accurate the calibration. you will notice that Mach 3 uses about 8 decimal places, so you need to be as deadly as possible as well. You need to get some local help from a machinist or a machine shop. Talk to them and see if they will give or sell you a piece of steel bar stock, say likely a piece of 1/2" square cold rolled steel. Ask them to machine the ends smooth for you at about 11" long. Once that is done ask them to measure, accurately the actual length of the bar, to the closest .001" or even to the closest half thousandth. Now you know the length of the bar - exactly. Keep in mind that the length of the bar will change with the temperature of the room (time of year - winter summer).

It is important that you know the exact length of the bar. I doesnt matter what it is but you then need to vibropeen that dimension into the bar so you dont ever lose the size. The bar can even be 11.379" long, you only need to tell Mach 3 how much to move, so add the bar length and .500" and put that into Mach 3.

Ok, now repeat the calibration process, however this time use the steel bar as a spacer between the machine and the tip of the dial indicator. now when you tell Mach 3 to move the machine, tell it to move the machine 11.500" (or the bar length plus 0.500"). this will move the machine and only depress the dial indicator 1/2 of the travel. But now you are calibrating the machine over a longer distance and this process will be MUCH more accurate.

If you find the the machine moves more or less than you expect then just calculate that distance and add or subtract it from the 11.500" you expected and put the new length into Mach 3 and it will do the math and update your steps per inch for you.

Once you are all finished and everything is working accurately - get a note book and WRITE the number of steps per inch, for each axiis into the book and you shouldnt ever need to do this again unless you make changes to the machine. In fact make sure you record ALL your Mach 3 calibration information. You can do that for EVERY Mach 3 screen by pressing CTRL/Print Screen - and print out every screen using Paint, and put them in a binder..... put a date on each page..... keep this so you dont lose it. way easier than writing it all down. Also make a copy of your Mach 3 .xml configuration file and rename it so you dont lose it either.

Make sure you have NO backlash on your machine anyplace as that will screw you up badly. However if you do have backlash, there is a place in Mach 3 where you can tell Mach 3 what your backlash is, and it will automatically adjust it's movements to compensate for the backlash. I have never had to do this so I dont know how well that works, but that option is available.

Peter,
Calgary Alberta.

ElevationCreations
Vectric Craftsman
Posts: 130
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Vcarve Inlays not Locking?

Post by ElevationCreations »

Peter,
This is a great method for calibrating the steps.

The Circle Diamond Square test is used to identify if the machine is square, as well as check the accuracy of the machine.

Do you have a method using the dial indicator to check for square?

Peter Stenabaugh
Vectric Craftsman
Posts: 189
Joined: Wed Jun 07, 2006 7:26 pm
Location: Calgary, Alberta Canada

Re: Vcarve Inlays not Locking?

Post by Peter Stenabaugh »

Unfortunately I do not, at least using the dial indicator. However one process that can be used would be to cut a square hole, then cut a square insert to fit the hole, much as if you were making an inlay, but dont use the inlay process, just cut the 2 parts. then take the insert piece and flip it over left to right. If the machine is cutting square the edges will fit perfectly - similar process to checking for a square cut on a table saw. By flipping the part over, if there is any 'out of squareness' the gap shown will be TWICE what the error actually is, since you are seeing the error as shown by both parts at the same time.

I have made myself a large 'square' using some aluminum flat bar. I have 2 pieces about 3' and 4' long which are joined at one end with as single nut and bolt. Then I have a longer (approx 5') bar that is attached as the hypotenuse of the triangle. (3' x 4' x 5' is a perfect right angle), but any size works. I set this up so that one end of the 5' bar is bolted and screwed but the other end is fastened with a small slot so that I can set the jig up to be as square as possible. This hangs on the wall to be used as required to check the squareness of the gantry against the frame of the machine's X axis. My cutting area is 48 x 78 so I made the jig fairly large to fit the machine. To set the jig square, I use the factory edges of a piece of plywood or something like that as a master template. This probably isnt perfect but it gets my router as square as possible.

With the gantry set as square as possible, you can then cut a groove in the top of your router table about 1/2" deep x 1/2" wide (or whatever works best) and then insert 2 strips of baltic birch, or lexan plastic or whatever you have around the shop so they stick up about 1/2" above the top of the table. This then gives you a 'fence' which you can use to help align things for setups. Leave the strips loose so they can be removed if need be. Cut the 2 grooves about 3/4 the way across the table in both directions.

Another option is just to secure 2 strips of 1/2" thick material to the table in place of the grooves, and adjust them to square and hold them in place with a few screws, but if you need to remove them for some reason you have to piddle around and set them up again......

Different strokes for different folks..... several ways to look at it.

The circle diamond method is ok for most things, but the big issue is that it is really difficult to get an ACCURATE measurement on a piece of wood, using a set of calipers. I always work to .001" even when doing woodworking, when I can, I guess I am just so used to machining metal I figure i should be able to get the same accuracy from wood, although I never do..... :(

The calibration in Mach 3 has to be done as accurately as possible, so you get out of it what you put into it..... wood isnt an exacting science but I try to make things as accurate as I can, then when I screw things up - which happens a lot - my mistakes are sometimes recoverable.....

Pete

Post Reply