FreeCad Inlay (Part 2)

 This post will be using the SVG saved as Base in Part 1.

Click image to enlarge

This post will be focused on the red base in the image above.  The same 60 degree v-bit from Part 1 is used.  Take note of the 0.100" depth of cut,  the 0.050" prismatic over-cut,  and the small green triangle representing the prismatic offset.  There is a note mentioning sanding to create the other gap shown but I haven't found this to be necessary in practice.

Oh No ! It's trigonometry !

    The triangle on the left represents the green triangle in the sketch above.  To achieve the .050" gap the perimeter of the Base pocket needs to be inset 0.029"

tan30 * 0.050 = 0.029

The tool path for the v-cutter also needs to be inset.  In the image to the left the blue triangle represents the material the cutter will be removing removing to achieve a 0.100" depth of cut.

tan30 * 0.100 = 0.0577

0.0577 * 2 = 0.1155

0.1155" is the full width of cut

 

 

 

A description of what happens next

The image on the left is the Base SVG modified for illustration purposes.  The thin green outer border represents the full size of the Base SVG.  This green border is 0.029" wide and will be deleted.  The red represents the 0.1155" wide v-carve cut.  The green area in the interior will be removed in a clearing operation.

 

 

 

 

Yikes ! It's Inkscape !

Inkscape 0.91 is used here. 

You were warned this was coming in Part 1.  The Base SVG is modified here.  Get rid of any fill and apply a stroke if necessary.  Set document properties to inches.

1  Edit -> Preferences -> Behaviour -> Steps.  Change Inset/Outset  to 0.029"

2  Select the path outline and then apply Path -> Inset.  This will be the pocket perimeter.

3  Return to Preferences and change the steps to 0.1155"

4  Make a duplicate of the current path.

5  Apply Path -> Inset

6  Select the outside path and apply a black fill.  The SVG should now look like a solid black diamond.

7  Ctrl + A to select all.

8  Path -> Difference.  If all went well there should be a black diamond perimeter with a white centre.

9  Save the file as an Inkscape SVG

Finally FreeCad Time

1  Import the SVG into the Draft Workbench

2  Select the outside path then the inside path.  These may be a bit obscured.

3  Modify -> downgrade to create a cut.

4  Repeat Modify -> downgrade to create a face.

 

This post got too long.  Continued in Part 3     
 

FreeCad Inlay (Part 1)

This is a continuation of the previous v-bit post.  Please scan that first.

Disclaimer:  I am new to FreeCad.  There may be easier ways to do many of the things shown in this post.  FC v0.19 pre-release is being used in this post.

The SVG file used was downloaded from wikimedia.  I believe it's this https://commons.wikimedia.org/wiki/File:SuitDiamonds.svg 

 

Save 2 copies of the SVG file naming one Inlay and the other Base.  In this post the copy named Inlay will be used. 

Click image for larger size

In the image above the red base piece is cut to a depth of 0.100".  The aqua inlay piece is cut to a depth of 0.150".  The aqua part is being made in this post.

Making the inlay

1  Import the SVG into FreeCad Draft Workbench. (toggle off that annoying grid).  Use Modification -> upgrade to create a face.  This seems to work best if the fill is first removed in Inkscape.  If anyone tries to follow along without a knowledge of Inkscape things will get worse in Inlay (Part 2).  The SVG should be flipped horizontally in Inkscape before importing.  In this case the SVG is most likely symmetrical,  the point is inlays must be a mirror image of the base.

2  Open the Part Workbench and extrude the face to a thickness of 0.150".  In the extrude dialogue box skip Apply and hit OK.  Apply creates a redundant copy.

3  Create a cube the length and width of the stock material being used for the inlay.  Height isn't critical but the actual stock thickness minus 0.150" would be a logical choice.  Place the cube in the appropriate x-y position beneath the extrusion.  Lower the cube's z position by an amount equal to the cube's height.  If this went well there will be no gap between the pieces and the extrusion will protrude 0.150" from the top face of the cube.

4  Click on the extrusion and the cube and create a boolean union.  This should result in a single object named fusion.

5   Open the Path Workbench.  When creating the Job choose Fusion 0 in the first dialogue box.

6  In Job set-up window make the top of the stock level with the top of the model.  If any facing is needed take care of it beforehand.

7 For this operation a 0.250" tool controller was used.

8  Use a pocket tool path to clear the area around the diamond to a final depth of 0.150".  If this is done right the diamond shape should be all that remains of the original top surface.

9  Using a profile op cut around the perimeter of the diamond to a final depth of 0.150".  Adjust the step downs to something sane like 0.050".  In the profile operation deselect "Use Compensation".  The logical operation to profile the diamond is the engrave tool path but it's approximation of the curves was too crude.

10  Post the tool paths. Order of operations should be pocket followed by profile.

11  When cutting the profile tool path use a 60 degree v-bit in place of the 0.250" end mill. 

This was the easy half to explain.

Part 2 gets messier.
 

FreeCad and V-bits

 This year has brought changes to Autodesk's free subscriptions.  These changes along with a general dislike of software as a service have me looking for a Fusion 360 alternative.  I gave FreeCad a brief look in the past but the CAM tools were too limited for some of my projects.  FC v0.19 is now near official release with a larger variety of tool path operations.  Some bugs remain and some things are a bit clumsy but it's becoming a legitimate alternative.  

The Path workbench creates the everyday tool paths in the usual kind of way and these are reasonably well documented.  In an effort to better understand FreeCad I'm testing some of the less commonly used path tools.  My experiments will be recorded here as notes to myself.  If they are useful to anyone else you're welcome and thanks for reading.

First up is the v-carve operation but not used in the way FreeCad intended.  The goal is combining v-carve with other tool paths to create inlays using the methods employed by F-engrave.  This has been an adventure and my respect for F-engrave has increased in the process.  This is no knock on FreeCad, Scorch's software is specialized and what it does it does very well.

FreeCad's v-carve tool path works on the concept of fitting a circular diameter to a face shape of various widths.  For example a face width of 0.100" will require a 60 degree v-bit to a depth of 0.0866".

The math in this example is pretty basic.

(0.100/2) / tan30 = 0.0866

and at full depth

(0.250/2) / tan30 = 0.2165

These numbers describe a 0.25" 60 degree v-bit

The description above is of course an over simplified description of the concept.  I believe in reality some fancy math is used involving something called Voronoi Nodes. 

Testing the numbers above on a 0.100" wide face returned weird results.  I discovered that the tool editor has bad labelling for the included angle definition.  To properly describe a 60 degree included angle cutter the value to enter in the tool editor is 120.

The math is 180 - included_angle.  ***

Another oddity, possibly connected to the glitch above,  is the connection between tool diameter and depth of cut limit.  To enable full depth of cut the tool diameter must be defined larger than actual size.   Watch out for this if intending deep cuts.

*** FC v0.19 will have a new tool bit system so these problems may only apply to the legacy tool system.  The release of v0.19 is expected by the end of 2020.

The v-carve operation includes options Discretize, Threshold and Tolerance.  I have been unable to find good definitions for these options and they may not be fully developed at this time.  The FC wiki has an example of using v-carve but these options are not described there.

Are inlays possible using FreeCad ?

Yes and No.

That's the next post.                                                   

Inlays with F-engrave

F-engrave 1.73 is being used in this blog post.  The YouTube videos are excellent but the gui has changed enough to need a bit of explanation.

If using linuxcnc: settings -> general settings -> un-check 'suppress comments' can be useful.

Click on any image to enlarge.

The dxf file is a simple set of rectangles.

The main items of interest are the image height and the v-carve selection checked.

In General Settings you may want to enable center format arcs.

The origin is set to center in this example.

Settings used as shown.

Calculate v-carve.

Calculate clean-up.

Save clean-up gcode.

Save v-clean-up gcode.

In this example cuts were deep enough that no clean-up was needed.

Close settings window.

File menu -> save gcode as "name"_female.  This is the v-carve tool path.

Next...

Mirror image.

Re-open v-carve settings.

Check 'add box' and 'prismatic'

Set gap, in this example 1/16"  (-0.0625)

Calculate v-carve.

Calculate clean-up.

Save clean-up g-code

Save v-clean-up gcode.

Close vcarve settings window.

In main window: File menu -> save gcode

Save as "name"_male.  This is the male v-carve path.

There will be up to 6 g-code files.  If using a tool change routine or a tool changer this can be reduced to 2 files using the Linux cat command.  Remove unneeded M2's and add T# and M6's as needed.

For illustration purposes STL files were created using Camotics.

Meshmixer was used to mate the 2 STL files.  The result was brought into QCad to add the dimensions.  If the result isn't exact to the decimal place blame the weird mix of software.  The gap is very close to the intended 0.0625".  This gap provides space for a saw blade between the 2 surfaces.  See why sanding away the pointy tops of the male part before clamping/gluing is a good idea ?

A small note on using F-engrave for inlays: the software calculations are based on a cutter with a true point.  If the cutter has any amount of flat on the end the tool height must be adjusted accordingly.  Even a flat of 0.030" can result in a failed inlay.  Other pit-falls are an off-center cutter point,  a spindle with run-out, and v-bits labelled with a  nominal (not exact) included angle

First Try at a Lithophane

 

The creator of the image above posted it to an internet forum.  I'm assuming it was provided for free use for non-commercial purposes.  This type of image is ideal for creating a lithophane.  Unlike like some of the finely detailed lithophanes posted elsewhere this image won't require micro sized cutting tools or endless hours of cutting.

Recently I've found a source of Corian cut-offs at near give away prices.  Corian is a brand name Solid Surface Material which has translucent properties if not infused with dark pigments.  The piece used in this post is some shade of white.

   To get the lithophane effect the Corian was first milled down to a thickness of 0.130".  As shown in the screenshot above the 1/8" ball end mill will be carving to a max depth of  -0.100 which means only 0.030" of material will remain at the deepest parts of the carving.  The settings shown in the image above are the exact settings used.  A roughing pass was also used but is not shown here.

Camotics was used to check the gcode before cutting.  Camotics can be a bit deceptive depending on how the image view is rotated.  The first image shows the features on the chin a forehead as depressions:

in fact they stand proud of the surface as shown from this angle:

Below is the finished item back lit with a florescent light which makes it appear quite yellow.  When illuminated by natural light, such as hung in a window,  it has a bluish-white hue which I find more attractive but more difficult to photograph.

More Wooden Toys

This post is a fan tribute of sorts.

I've built several projects based on files shared by trinityscsp (Juarez) via GrabCad.  A few are pictured below.  Juarez, if you ever stumble across this site, thank you for your generosity.

Farm Truck

https://grabcad.com/library/old-farm-truck-1

Speedster

This one is a work in progress.  Still looking for suitable material to make the fenders
https://grabcad.com/library/speedster-wooden-toy-1

Sports Car

https://grabcad.com/library/sports-car-wooden-toy-1

Buggies

https://grabcad.com/library/baja-buggy-wooden-toy-1

All together with the truck hauling a 2 litre bottle for a sense of scale.
The camera seems to be adding some amount of a distorted perspective to all of today's photos  but I've never claimed to be a photographer of any skill.

Easy Name Puzzle

If you have a CNC router this personalized gift is an easy make. This project uses maple for the letters and Baltic birch ply for the cat and base. The font used is 'Life is Goofy' downloaded from one of the popular free font websites. This font was chosen for ease of cutting and to my eye it looks like something that would feel good to a toddlers hands. The cat was a Jpeg named 'peeking cat' found with a Google image search.

Inkscape was used for most of the design work.  I'll assume if you want to duplicate this project you already know how Inkscape handles bitmaps and fonts. If that's assuming too much the internet has plenty of tutorials on those topics.

The puzzle pieces should be a slightly loose fit unless the toddler is being provided with a hammer 👶.  To achieve this fit Inkscape's Linked Offset feature was used along with Guidelines to measure the amount of offset.  The Offset in this case was actually an inset of approx 0.025".  For the puzzle pieces delete the original outline (aka path) and save the inset. Save the original outline (aka path) as a separate file for cutting the pockets. 

The work in Inkscape results in 4 svg files:
#1 cat svg non-offset for pocket
#2 letters svg non-offset for pockets
#3 cat svg offset (inset) for puzzle piece
#4 letters svg offset (inset) for puzzle pieces

These 4 svg files are imported into Fusion 360.

Create the plywood base in Fusion 360.  Import and align svg files #1 and #2.  These files are cut with a pocketing tool path.  Outside contour  the base to it's final shape.

Create another file in Fusion and import svg file #3.  Cut the cat with an outside contour tool path.  Follow the same procedure for svg file #4 to create the letters.

The puzzle pieces should protrude far enough above the base surface to allow grasping by little fingers.  Paint the puzzle pieces on the top side only.  This will reduce confusion with those letters which appear to be reversible.

Btw: Fusion 360 can occasionally be stubborn when trying to extrude imported svg files.  If this happens try converting the svg to dxf using QCad.