Good afternoon all,
Hope to find you safe and sound.
I’ve been working on a project in which I need to transfer a board design from BoardCAD into Fusion360 so I can further edit its volume.
I’ve tried to export in different formats but nothing seems to work.
Any help would be greatly appreciated!
Many thanks
Jo
Hello Jo,
Have you seen this thread?
https://www.swaylocks.com/forums/help-boardcad
I have not found an easy way to go from BoardCAD to Fusion360.
You could take the DXF sections from BoardCAD you could bring them in as sketches into Fusion and then re-loft the board and then change it as you see fit.
STL might also be a possibility, I have used this to go to other software but the facets were not a concern for that project.
Here is a video from Autodesk on using a mesh body like STL to create a surfboard object in Fusion360:
Since my primary board shaping tool is hotwire on EPS foarm followed by planing and sanding, the outline and rocker (profile) templates from BoardCAD work well for me.
These I either print on paper, tape together, and cut out with a scissors or if I have the time or mood I will convert them into a file to be used on a CNC router or laser.
If you discover a better method, please let us know here in General Discussion.
Good evening J.
Thanks for your reply and your help.
I’ve just uploaded DXF files of the outline, profile and various sections into Fusion but I’m having some difficulty on extracting them from the plans (into which gets uploaded automatically) so I can manipulate them. Any idea on how to solve this?
Once again, thanks for taking your time to help me here.
I’m trying to find other ways to sort this. I’ve I accomplish it I will share them as well! 
Cheers
Jo
Hey Jo,
I try to set up a sketch for each section, and one for prodile and one for outline. By using the pfofile and outline you can make a blank. By having accruate sections you can begin to define a board’s shape.
Does you session look like this?
Good morning J,
It looks great! The trouble I had in fusion is that I cannot select neither sections or outline or profile into a face, so I can sketch them. I did then try to do it in AutoCAD and the result was similar to what you have. Could you explain how you managed to get the plans in Fusion?
Good Afternoon Jo,
You are getting close. Remember that I said it was not easy…
The idea is to have a simple DXF for each sketch in Fusion, and import the DXF files one at a time into the correct sketch.
One DXF for plan, one for profile, one each for each section.The output of BoardCAD should allow for a one at a time.
What makes it challenging is tha it is up to you to align the simple sketches in the correct locations in space in Fusion.
This is where the shaping softwares have more power than regular CAD’s is that they specifically keeps all of these pieces aligned naturally.
If you outline is in the XY plane, the profile should be in a sketch that is in the XZ plane and each section will be in its own YZ plan that is offset in X to match the section positions in BoardCAD.
So next step is to add the profile into its own plane. Out of time to add more this morning…
Actually I do not understand the problem, because you can edit the volume in BordCad quite easily by changing dimensions or the curves of Outline, Profile and Ribs.
If your problem is to get finally a good printout, for HWS I suggest the Hollow Wood Template Maker by Jedail…
It might work to organize the BoardCAD info into a single drawing/DXF like this. Remember that there is ususally a small gap in the polyline from BoardCAD that will need to be fixed before Fusion will allow lofting. You will also need to know the ‘altitude’ of the sections and rocker to place them correctly.
Hi,
Thanks for your imput.
What I intend to achieve is something similar to the picture attached. Getting a full 3D surfboard template in Fusion360 or AutoCAD (not quite sure which one is best for this) and then remove internal volume to remove weight.
Hope this makes sense.
Best regards,
Hi J.,
Thanks for your help.
Still struggling a bit on turning the DXF files from vectors to faces (as last picture).
Any difference between AutoCAD Mechanical and regular AutoCAD to do this?
Thanks alot for your help.
Regards,
Jo
Did you close the small gaps in the sketches? Normally happens near x0,y0 of the original DXF from BoardCAD. The last segment to close is missing.
If Fusion detects a closed outline, it shades in blue and becomes available for extrude, loft, sweep.
Same file as before read into Fusion after gaps were closed, scaled into inches, and sections moved as shown with a telltale for rocker. Otherwise the sections come in at 0,0 without the rocker value added.
BoardCAD does volume natively. If you correct for foam density or average density for HWS you should be pretty close.
It looks to me, that you do not want to reduce volume, which is given by the hull, but the specifiic weight of the volume, to finally reduce weight. But this may be solved without any CAD, just compare the weights of foam, wood or that hexagon structure for the same volume and you are solved. You can even calculate the hexagon structrue with a calculator.
And the use board cad weight estimator…
This is a picture of as far as I can take this.
BoardCAD DXF’s output for outline, profile, and 3 sections in the tail.
Oriented as shown earlier. Probably would have been best to replact polylines with splines to reduce entity count.
Brought into Fusion360 and placed into appropriate sketches.
Body 1 (light gray) is the ‘blank’, extruded from the outline and trimmed by the profile, sketches 1 and 3.
Body 2 is a simple loft between 3 tail sections, sketches 5,10, and 12. I did replace polylines with spline here otherwise Fusion would crash from 1000’s of small segments.
Next step would be to add remaining sections and redraw the profile as splines and use it as a ‘rail’ for the loft to better acheive design thickness distribution…
It would be faster for me to make a board by hand than to draw a board this way in a parametric CAD system.
I do like Fusion360 as a software, but I prefer BoardCAD for the board design and hands-on the materials for the rest.
Good morning J,
I thought I had replied a couple of days ago but I believe the message didn’t get saved, for some reason.
Thanks for your help. The work you’ve got there looks amazing.
I’ve been trying to get Splines to replace the Polylines as everytime I try to use the command Loft or Sweep in Fusion, this crashes as you mentioned before, but neither AutoCAD orr Fusion are reading the this file (creates a PDF file when imported to Fusion?).
I was wondering if you could share the tail that you’ve made in Fusion so I can check the timeline and hopefully overcame and understand all steps that need to be done.
Due to the materials I’m gonna be using to produce this board, it needs to be drawn and shaped in CNC rather than by hand.
Thanks again for your help,
A public link to the design so far, sharing is caring and all of that jazz (I do appreciate all I have learned at Sway’s):
Jo, looking at your pictures, you might be creating bodies early, forming ribs so to speak.
From my timeline:
Sketch for outline, import DXF, remove extra entities, replace with splines if desired
Sketch for rocker, import DXF, remove extra entities
extrude oultine
extrude rocker+extra rectangle (cut) to form ‘blank’ body1
Create work plane for each section, same offset as sections are in BoardCAD
Create sketch for each section on its work plane
-import first tail section as dxf draw splines over polylines and erase polylines 1/2 of section only to save time and lower entity count. Sections need to be at same ‘altitude’ as profle
-import second tail section same as above
-inport third tail section same as above
Loft section sketches to form second body. If profile is a clean spline use it as a rail or guide for lofting
Mirror solid over to form second half (not shown)
Let us know if this helps.
