VCarve Inlay - ALMOST there!

[davekenyon]

Hi Russell

Thanks for the reply. I've run a test piece and my v-bit may be less than 60 degrees.

Upon very close inspection, what's most concerning is that all the corners seem to be 'stretched' in the negative-X direction (ie to the left in the picture). This ties in with the errors in my inlay pieces - corners cutting too deeply when cutting on the left-hand side of the cutter and not deep enough when cutting on the right.

Am I looking at the z-axis / spindle misaligned or (hopefully!) something less serious?

[Paul Z]

Russell's advise is dead on. See http://www.vectric.com/forum/viewtopic.php?f=3&t=2164.
It gives you an idea of what to look for.

Once you discover the angle, keep that one in your tool data base and use it whenever you use the bit.

If some corners look ok and others don't, it is likely that your tool is not perpendicular to the table. If so, your router/spindle needs to be adjusted to be parallel to the Z axis on your machine and the Z axis needs to be adjusted to be perpendicular to the table. The last step is much easier if you use or make a trammel. The trammel "magnifies" any misalignment. If you have a 1/8 collet, you can make a trammel from a piece of 1/8 music wire. The angles bent into the wire need not be accurate. The trammel is going to be revolved (BY HAND!!!) around the axis of rotation of the router/spindle. Once you have made adjustments to where the trammel just touches the table for 360 degrees, you are done and very accurate.

Paul Z

[davekenyon]

Thanks Paul

I suspect that misalignment is the problem. I'm going to be away with work for the next couple of weeks and will have a crack at it when I return. I'll have a scan around for some shims!

Dave

[Paul Z]

You may not need shims. Usually you can correct the alignment by loosening bolts, apply pressure and retighten.

Paul Z

[davekenyon]

I'll have a go at that first then Paul. I may have made things worse over the last couple of days - tightened everything to the max!

[copperhead4321]

you might try cutting a softer material like MDF it looks like you're cutting oak, see if you you get better results w/ mdf/ just a suggestion

[davekenyon]

Will try that - all good tips thanks!

[davekenyon]

Sorry to resurrect this but I’ve been away with work and have only just got around to following the advice.

The short version is that, after spending ALL day on it…. I still have the problem!

As everybody has said, it must be a machine / Mach3 issue. I’ve tried all sorts but I still get the little kinks, shown in the attached image. For example, look at the first ‘thick’ stroke – a kink inwards on the left at the bottom, and another from the right at the top.

Everything looks fine until the later cuts which also involve the Z-axis.

Here’s what I’ve tried so far (stumbling blindly!):

Adjusted all axes for sqaure – found a bit of misalignment but not a lot – removed with shims
Resurfaced the table - found a slight bow – now removed
Used a trammel set up to set the spindle perpendicular to the bed (great tip thanks!)
Tried reducing the feed rates (down to 5mm/sec and 1mm/sec plunge)
Made the cuts in MDF
Tried various Mach3 ‘step’ settings for the Z-axis (changed the depth of cut but kinks remained)
Recalibrated all motors
Reduced the acceleration in motor tuning
CV mode / Exact stop
Absolute / Inc distance modes
Absolute / Inc IJ modes
Backlash is disabled in Mach3 – tried settings of 0.01mm in all axes but had no impact
Rotated the toolpath 90 degrees – kinks remained in the exact same positions
Tried various v-bit angles (the best fit seems to be 56 degrees although the kinks remained! Interestingly, when I cut the pockets to determine this as advised all the corners seem to be ‘pushed’ in the negative x-direction. This ties in with the kink at the bottom of my thick stroke, which is in the positive x-direction! This makes me think that the kinks are being commanded.)

I’m completely stumped and desperate for any advice. Thanks for your time.

[P.Passuello]

Sorry to hear about your problems with getting the VCarve inlay to work.
My initial thoughts about what I see in the photo is it is either the angle of the cutter does not match the setting you have in VCarve Pro or you may have an issue with loosing steps on the Z axis.
The best thing to do with finding causes of issues is to try and come up with tests that will prove or disprove some aspect of the issue you are having.
Here is how I would approach it.
First confirm cutter angle, which I see you have already done. The test cut shows it is 56 degrees (unless you have changed cutters), so use that figure in VCarve Pro to make your files. Your photo indicates you used 54 degrees and the result is what I would expect to see if the angle used in VCarve Pro was smaller than the actual cutter.

If in any doubt re-cut your tool checking file to make sure you haven't accidentally grabbed a different cutter by mistake.

You are concerned that the Gcode is causing the strange cut and of course anything is possible but it is very unlikely to be a VCarve Pro issue. However do double check the angle of your cutter is set correctly for the cutter you have chosen. eg Just because the tool is called 56 degrees doesn't mean it is set 56 degrees in the tools profile. Feel free to post your CRV file here of a second opinion. The fresh eye can sometimes see at a glance what hours of staring at can miss. Been there, done that.

Check you are not losing steps on the X Y or Z
Your steppers are double shafted so it is really easy to do.
Once you have set your 0,0,0 position in Mach3 get a felt pen and draw a line on the shaft down onto the body of each stepper on the back. When you finish the cut return to origin and make sure the lines match up again. If they don't you have lost steps. You can put masking tape on the motor body to mark if you prefer.

I would personally use exact stop for all test cuts since constant velocity does not follow the gcode exactly but does an approximate cut. I don't think this is your problem but turn CV on when you have solved the issue.

I see what you mean about the scallops being off to one side on the X direction but I see them on both the +X as well as -X which makes me think the cutter angle is wrong or the Z is loosing steps. I also see it in the Y direction in the corners of the square.

Long story short:
Triple check your VCarve pro file and make new Gcode file.
Double check the cutter.
Cut new file and when finished check you haven't lost steps using marks on the motor shafts and visually check your cutter position in case you have lost exactly 1 full revolution of the stepper. (Very unlikely but Murphy likes to play tricks)
Post photo of new cut.

Hope this helps
Peter

[davekenyon]

Hi Peter

Thanks for the response. I'm away with work again tomorrow so the speedy reply was much appreciated!

I've attached my CRV and Mach files. Last cut was with 'Exact stop' selected. I've not posted a photo of the cut, instead I've attached a photo of the Z-axis after the cut. Great bit of detective works thanks Peter! Looks like I am indeed losing steps in Z (X and Y were spot on).

The next question might be a bit basic for most people, but.... how do I cure it?

Thanks
Dave

[P.Passuello]

Excellent, you are half way there.

Could you let us know what driver you are using to drive the stepper motors and are you driving them straight from a PC parallel port or are you using an external step generator like a smooth stepper or similar?

Unfortunately the Aspire files are of no use to me as I only have VCarve Pro but others will be able to confirm that it is correct. The text file is only useful to someone with a 56 degree cutter. Having said that you are clearly loosing steps on the Z so we'll fix the obvious first then worry about the rest if it is a problem.

Cheers
Peter

[Mike E]

I noticed in your Mach3 settings your "Line Look Ahead" was set a 20. I had much smoother operation setting at 200. Also I "Constant velocity" but turn off the cv options.

Good Luck
Mike

[davekenyon]

Mike - thanks for that. Will alter the setting - surely can't do any harm?!

Peter - you're getting a bit advanced for me now! I've attached a picture which I took last time I had the cover off. Does this help? From what I remember, the box on the right runs to the laser attachment. Let me know if not and I'll do some rapid disassembly.

Thanks again
Dave

[davekenyon]

Low res only but they might help.

[P.Passuello]

To figure out the cause of lost steps will require quite a bit of info from you but as a general rule of thumb I would look at the motor tuning settings for the Z axis to start with.

There are 3 things in there that need attention.
Maximum speed - This may be set too high and will cause lost steps as the axis gets to top speed. (Try halving it)
Acceleration - This will have a huge effect and is very likely to cause lost steps if set too high. The motor will stall ass it tries to accelerate to top speed. (set to a low figure)
Pulse and direction time - These should be set to manufactures spec or greater. I would personally, for the purpose of testing, set both to 15 in Mach3 as it will not effect the machine but guarantee pulses are ok to the driver and remove pulse width as a factor. Change them back when you have finished testing.

Hope this helps.

Cheers
Peter