V-Engrave Help

[Spannerhappy]

Its a 1200mmx1200mm automationmaker machine with a watercooled 2.2kw spindle motor. I wasn't using the speed settings on cb as it runs on its own variable power source and seems comfortable at about 9500-10000rpm.  I find it strange that these errors seem to re-occur in nearly the same places. Should i be looking at the hardware? Can the micro-stepping drivers be at fault? The first attempt I made the machine worked left to right  and i have';t been able to replicate that. The single line text starts on the middle, moves to the right then jumps all about the last few letters. When I cut the 4 lines of text it starts at 47 then almost cuts random letter to random letter with no obvious route. Maybe if i could get it to cut left to right i could reduce the error rate? Can i change the tool path?

[EddyCurrent]

I'll give your file a try on my machine tomorrow and see how it turns out, time permitting.

[EddyCurrent]

Here's the result of my test.

I used this tool; T107-1/2  , https://www.wealdentool.com/acatalog/Online_Catalogue_Engraving_90_Degree_718.html
running at 19000 RPM

Attached is the cb file used.

It cut the letters left to right with no jumping around.

So my question is, how are you setting zero for the Z azis ?

 

[Spannerhappy]

Hi Eddy, thanks for having a go. Strange its changed the font though? I set the Z axis by lowering it to the timber surface with a piece of paper between the cutter and timber. Then I can feel the resistance on the paper to call zero.
My problem is i bought this machine second hand with a promise that it works and its my first experience of using it so there could be problems on software, post software setup or even hardware. The one thing clear is that my machine isn't cutting like others is so I better start looking again at the hardware.
 I find it strange that the letters themselves are always correct (not stretched or distorted) but the location of them isn't. I'm going to change the connector cable between the pc and machine controller and then see if there is a way to slow the movement from 1 letter to the next. Maybe thats where its loosing count of the movement?
Any idea why the Cambam software doesn't always start from left to right?
Thanks for your efforts to help

[dh42]

Hello

I find it strange that the letters themselves are always correct (not stretched or distorted) but the location of them isn't.

Not so strange ; there is a rapid move between each letters, and mostly it's with rapids that you can loose steps because it use the max torque at the higher velocity. (on a stepper motor, the torque decrease when the RPM increase)

In mach3, on the "settings" screen, there is a box where you can specify the rapids to use without to have to change anything in the motor tuning ; it is Rapid OvRd ; give it a rapid feed value lower than the one you've defined in the motor tuning, and click on the button to activate the overide (a LED will switch to green), then when you have find a suitable value for your machine, you can duplicate this feed in the velocity box in motor tuning and disable the overide (note: the rapid overide act only on the Gcode, with manual moves, the rapid still use the value in motor tuning)

++
David

edit: PS, always set the Max Depth of the V-engave to Auto to avoid deep cuts
https://cambamcnc.com/forum/index.php?topic=7910.msg63327#msg63327

[EddyCurrent]

The font shows as in the attached image but I don't have it installed, maybe you could use a standard Windows font for future tests.

CamBam does move about at times due to "Optimisation Mode", if you set it to "None" it will move to each object in the order they are listed in the MOP "Primitive ID's" list.

You could try this standard cnc test, https://timf.anansi-web.com/wp/circle-diamond-square/, it's in inches so convert to mm if need be and it can be easily drawn within CamBam.
Once that is cutting correctly you can move on.

edit: PS, always set the Max Depth of the V-engave to Auto to avoid deep cuts
https://cambamcnc.com/forum/index.php?topic=7910.msg63327#msg63327

It's a good tip, I've never used it myself because I always check depth of cut before actual cutting.

I can't remember if this has already been mentioned but there is a simulator here; https://camotics.org/
that works nicely with this plugin; http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/Simu_camotics.html

[Bubba]

What Eddy said is absolutely correct. Machine G0 moves are rapid travel and that's where your machine is loosing steps as I mentioned in my previous post. In Mach3 go to 'Config', 'Motor Tuning' and slow axis that causing problem about 10%, it don't take much to correct this. To gave you an idea what I'm talking about see the attachment. Good luck. 

[Dragonfly]

If you want to make the project portable across machines and retain the originally selected font convert the letters to poly lines. It will fix the missing font replacement by the OS.

[kjlpdx]

i suggest you buy some rigid pink foam insulation for practicing on first.  it cuts quickly and doesn't dull your bits much.

[Spannerhappy]

Thanks for all these helpful suggestions. I am making progress all be it slowly. While changing the serial connector for a new one I found some dodgy wiring at the main power board on the cnc machine. There were loose connections that might have caused some of the rapid movement loosing count as the power draw over a bad connection might have dropped the voltage significantly during these high speed passes. I've now fixed the connections, lowered the Rapid speed settings and changed the optimization settings to sensible! (thankyou for all these suggestions- its helped a lot).
The machine is now holding straight lines, carving in a sensible sequence (left to right) and not trying to achieve warp speed between cuts. I'm still having issues with heights as my machine seems to keep loosing calibration despite me remembering to press save. Annoyingly the first cut i did on his machine left the ends of the letters perfectly square but now i'm getting a w shape- must be height.
Is there a proper guide to using v-engrave? Just a decent explanation for each of the settings would help. For example finish and roughing setting-is "finish" a double pass and roughing a single pass? Simple things like that- my logic can interpret either the wrong way!  Even now I get lost and have to reference the internet search engines to find an answer the simplest inquiry which takes ages.
Things done wrong:
buying a second hand machine!
dodgy connections (tightened)
wrong setting on optimization (now changed)
wrong rapid speed setting (now changed)
old serial cable (now changed)
dodgy pc (now changed for a newer one)

Thanks again for the help.

[EddyCurrent]

There is no guide for v-engrave that I'm aware of but all the help you need is here, just ask specific questions and remember to attach a cb file that is causing problems.

Unless you are using a 3D or Lathe machining operation, the "finishing" and "roughing" parameter is for information only, it does nothing other than inform the user.

Every piece of material I cut starts with setting Z height, also following a tool change, it's a habit you need to get into.
If you look on ebay for example and search for "cnc zero" those are the very cheap zero setters but I use one without problems.
If you then search for "cnc height" you will get something more sophisticated.

[dh42]

Hello

There is a small help here
http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/Vengrave_doc_EN.html

++
David

[Spannerhappy]

Solved it! A stray wire was the fault! The breakout board was replaced before I got the machine with one from CNC4u. There was a single cable with a bit of tape over the end of it from the low voltage feed on the stepper motor drives left hanging there. A very useful friend said "Why don't we attach that to the power supply on the breakout board?" With nothing to loose and no big flash or bang when we connected it and the machine worked! (maybe that's why they sold it?)
I can now go back to Zero every time and no longer have wobbly or mis spaced letters. Best of all the router no longer tries to do its ostrich impression!
Many thanks to all the support from the forum.