Inlay using V-Engrave

[dh42]

Hello,

the only way to make it easier as far as I know is to turn it into a Plugin

No, you can use the Custom Script Plugin ; it's very nice for script you use mostly  

http://www.cambam.co.uk/forum/index.php?topic=4587.0

the plugin: http://www.cambam.co.uk/forum/index.php?action=dlattach;topic=4587.0;attach=11685

++
David

[EddyCurrent]

Yes, I did think about BaNoBi's plugin after I'd posted.

[eastcoast]

thanks!

I learned something new today.. as did some others..

 but good idea to hide emails.

You don't need any of that Google stuff, a simple script in CamBam will do it.


Here's a quick one I made from another script, I'm a bit short on time just now so I'll tidy it up later.
I think it's doing the maths right.

Edit: added tidy version but just seen some more calcs need adding  

Edit2: Right, that's it, v1.2. To be used while reading the excellent info provided by Bob

[hebsmadwi]

Hello all! Thanks for all the work on this everyone! I'm about to try this. I installed the script and ran the calculator, and now I have a question. The calculator results show the inlay offset as a negative and the substrate offset as a positive (at least on my installation ). Is that correct?
Thanks again!

[macbob]

Hi Hebsmadwi,

No, that sounds to me to be backwards.  Using the 'Offset' tool with a negative value creates a new set of polylines on the inside of the selected polyline, which is what you want for the substrate, not the inlay.  You must have a rogue minus sign somewhere!

Have another look at the first post of this thread and try plugging in numbers manually.  That should show up the issue.


Bob

[EddyCurrent]

I've just had a look at the script and it looks like the offsets are being sent to the wrong text boxes, in other words the script is in error.

offset1 = Math.Round(-1 *(math.tan(TA/2) * (IL + GG) * 2),4)
offset2 = Math.Round(math.tan(TA/2) * (SA + AG) * 2,4)

so offset1 is going to be negative
offset2 is going to be positive

then it's saying;

offset1 = inlay offset
offset2 = substrate offset

I can easy change it once we agree.

Edit: updated script added, also well spotted, hebsmadwi

[hebsmadwi]

Hello Again! I've been playing around with this a little. I did get it to work with a small square inlay. Moving on, I am trying a small heart-shape. My question is, when using the offset tool, some of the sharp points are rounded. Is there is a work-around for that?
Thanks!

[macbob]

I think this is expected!  Your basic shape may have sharp points (e.g. the top and bottom of the heart).  The offset tool will be a little way outside (or inside) your basic shape and will probably have rounded off corners.  The zone between the two shapes will be taken out by the V-engrave cutter, cutting right up to both lines.  The V-engrave path should find its way right into the sharp corners, rising to the surface of the material as necessary.

[Garyhlucas]

Some CNC controls have multiple corner options. Fadal for instance had a mode where an offset tool sweeps around a sharp outside corner in an arc with its center right at the corner. Another mode did outside corners by projecting the tool paths to where they meet and cutter comes to a complete stop then goes off in the new direction.

[elieheloua]

J'essaye de comprendre l'explication anglophone et leurs calculs.
Les résultats sont différents avec celui du dessin à l'échelle.
Voir fichier dxf et image jointe.
Le résultat "inlay offset" chiffre devrait être paramétrer au champs profondeur final -9.2388 au lieu de -12.7 ?
J'aimerai bien avoir l'explication avec les chiffres versus variable de cambam au niveau "inlay" et "subtrate".

Merci de votre attention.

(For english, se google translate please sorry)

[macbob]

Hi There Elleheloua,

Looking at your diagram, I would expect that you need to put the value of 9.2388 into the 'Inlay' field in the calculator.  It will then display the values for 'Inlay Offset' and 'Substrate Offset' needed to be used for the CamBam offset tool.

Tool Angle 60
Air Gap 5.461
Sanding 2.54
Inlay 9.2388
Glue Gap 2.54

The offsets are horizontal distances, in the plane of the surface.  The inlay value will be positive, since you want to carve around the outside of your shape.  The Substrate value will be negative.

Have another look at my diagram at the start of this thread.

I'm afraid that I am at work, so I cannot see your DXF file and I cannot run the calculator.  I hope this is helpful never-the-less.

Bob

[dh42]

Hello,

I try to understand too ... and I don't understand the value for Substrate offset .. on my drawing I find 2.31 instead 9.2376  .. bug in the script or bug in my drawing ?

++
David

[macbob]

Hi David,

I think that the calculator is right, and that on your diagram, the ranges marked 2.31 and 4.62 are right, but that these are each half the intended offset for use in the offset tool.  You are measuring from the Profile line to the point of the cutter; you need to go the same distance again to get to the other line that the V-cutter must follow.

Your "Inlay Offset" caption should be to the left of the Profile line and the offset itself should be 4.6188, as shown by the calculator.  This is twice the width of the arrows you actually have.  Where you do show "Inlay Offset", it should show "Substrate Offset" and the value should be -9.2376.  Again, the width of the arrows should be double.

if you look back to my original diagram, the places that you have marked correspond to the boundaries of the zone to be hogged out with a milling cutter, should this be needed ("Inlay Pocket Clearance" and "Substrate Pocket Clearance"). Actually, I made a slight overcut, allowing something for the width of the glue gap, but it is much the same thing.

I wish this stuff was easier to explain.  I believe my initial description is correct, but you need to be a lawyer or a computer to follow the description!  Sigh!

[dh42]

Hello Bob

I wish this stuff was easier to explain.  I believe my initial description is correct, but you need to be a lawyer or a computer to follow the description! 

Yes, certainly ..  ... but I don't understand why the offset must be the double ... 

Maybe I understand after a night's sleep .. 

++
David

[EddyCurrent]

Yes, certainly ..  ... but I don't understand why the offset must be the double ... 

Maybe I understand after a night's sleep .. 

++
David

The reason is this;

CamBam engrave MOP engraves with the tip of the cutter ON the line, but V-engrave MOP engraves with the tip of the cutter down the centre of 2 lines.

So in the attached picture you can see that the tip of the cutter is down the centre between zero offset and 4.6188, and down the centre between zero offset and -9.2376