Hi

I need to create models for various types of surfboard and kiteboard fins.. but I'm not sure where to start.

I imagine would need an outline shape, and a foil profile - but not sure how to get it to take that profile throughout the whole shape. 

I thought of lofting, but for that I'd need to know the foil for a few cross-sections - but I was rather hoping that TurboCad would have some function that could do this for me.

Any suggestions?

Thanks very much
Tim

Hi

I need to create models for various types of surfboard and kiteboard fins.. but I'm not sure where to start.

I imagine would need an outline shape, and a foil profile - but not sure how to get it to take that profile throughout the whole shape. 

I thought of lofting, but for that I'd need to know the foil for a few cross-sections - but I was rather hoping that TurboCad would have some function that could do this for me.

Any suggestions?

Thanks very much
Tim

I'd say you're on the right track, Tim, and that lofting is the way to go. If you have a single foil profile, you can place copies at various locations and rescale them as appropriate. In fact, that is likely to produce a smoother loft than if you created a new profile at each location.

Henry H

Henry H

Hi Henry
Thanks for that.

I've created the side profile (using top view), then after a bit of fiddling with construction lines, managed to create a foil (using a bezier curve, copied then joined - it's not a proper foil for this fin) profile on the top of the fin - so looking front on it's like a T.

Now, as suggested, I'd like to copy the top/foil profile, say 3 times, and have these scaled and positioned so there front and rear ends are exactly on the side profile.

I've managed to create 3 copies, but I'm really battling to figure out how to scale them and get them to sit perfectly between the side profile lines.  I've create construction lines horizontally in the 3 places I'd like these foil profiles - hoping I'd simply be able to Edit, then drag to resize using a snap on the intersection of the construction line and the side profile - but this didnt work (moved or resized the foils incorrectly).

How should I do this?  I would have hoped there was some facility for doing this sort of thing.  I've been through the 2D and 3D tutorials and the reference manual but can't find anything that helps with this sort of thing - which I find odd - as I'd imagine it's a very common engineering task.

Thanks very much
Tim Huffam

Now, as suggested, I'd like to copy the top/foil profile, say 3 times, and have these scaled and positioned so there front and rear ends are exactly on the side profile.

I've managed to create 3 copies, but I'm really battling to figure out how to scale them and get them to sit perfectly between the side profile lines.  I've create construction lines horizontally in the 3 places I'd like these foil profiles - hoping I'd simply be able to Edit, then drag to resize using a snap on the intersection of the construction line and the side profile - but this didnt work (moved or resized the foils incorrectly).

How should I do this?  I would have hoped there was some facility for doing this sort of thing.  I've been through the 2D and 3D tutorials and the reference manual but can't find anything that helps with this sort of thing - which I find odd - as I'd imagine it's a very common engineering task.

No doubt there are at least nineteen different ways to do that, Tim, but I always find myself doing it by trial and error. However, here's a reasonably precise method...

To determine the required dimension of a relocated lofting profile, you could draw a regular line where the Construction line is now and use the Trim tool to make this line fit precisely within the side profile lines. Then select the trimmed line and read its Length in the Selection Info palette. Rescale your lofting profile to that same length. You'll probably need to rescale its width, too, using either a similar method or T&E or maybe an even better procedure of your own devising.

Henry H

Thanks for pointing me in the right direction.

I've got it looking pretty good now.   I'm staggered that in this day and age a modern cad program requires me to write down x/y offsets!

Now the profiles are in place... I've tried to loft.. from top foil profile to the bottom edge.. problem is it does not like the bottom edge - it will loft the profiles (which have 2 sides/eg an ellipse/airfoil) - but not from the bottom profile to the bottom edge which is just a single curved line.

Is there are way of doing this?  I'm assuming it cannot map both foil sides down to one edge - if so maybe I need to cut the foils in half and do one side at a time.

Thanks for pointing me in the right direction.

I've got it looking pretty good now.   I'm staggered that in this day and age a modern cad program requires me to write down x/y offsets!

Now the profiles are in place... I've tried to loft.. from top foil profile to the bottom edge.. problem is it does not like the bottom edge - it will loft the profiles (which have 2 sides/eg an ellipse/airfoil) - but not from the bottom profile to the bottom edge which is just a single curved line.

Is there are way of doing this?  I'm assuming it cannot map both foil sides down to one edge - if so maybe I need to cut the foils in half and do one side at a time.

Sounds like a problem I encounter often and for which I've never found an elegant solution. Try this: Instead of using just a single curved line for the bottom edge, put one or two more copies of your "airfoil" profiles down near the bottom, and rescale them to fit your side profiles. The lowermost "airfoil" can be made very tiny -- small enough that the finished loft will look fine from any reasonable viewing distance.

Attached screenshot shows a hasty example.

Henry H

Surfboard fins traditionally have a "shark fin" shape and are usually molded as if cut from a sheet with sharpened leading and trailing edges.  Using a "shark fin" shape, if the fin's thickness is constant, the aspect ratio of the section varies.  If the aspect ratio is constant, there's a variable taper.  If the foil section is a formal definition that you want to maintain, but with a shark fin shape, it might be more workable to space scaled profiles along a line corresponding to the thickest section of the chord, like the taper of a traditional airplane wing, then stagger/space them along a curve iteratively to find which arrangement most closely corresponds to the shark fin shape you want to achieve.    It's also simple to derive scaled profiles from a simple tapered model that you can pass sections through for local subdivision of the loft.  It seems most likely to me that you'd need sharp (discontinuous) leading and trailing edges, and without the necessity for side-to-side continuity across the change of direction, it's simpler to model one side and mirror it when you're satisfied with one side's parameters.

Shark-fin airfoil...

One Spline by Control Points; mirror-copied; four additional copies of the pair relocated and rescaled; the works lofted with "Use compound profile" enabled.

Henry H

Thanks guys for your help - I really appreciate this!

Yes, usually surfboard fins (my next project after the kiteboard fin) have a known foil shape.  Kiteboard fins, from my observation, have less of a proper foil shape - usually because they have to accomodate 2 screw holes and are very shallow.

Both kite and surfboard fins would have a leading edge that's more rounded (although very narrow) and with a sharp/fine trailing edge.

The kiteboard front-on profile is somewhat parabolic - maintaining it's diameter through much of it's depth, tapering more at about 2/3's of it's depth.

I've attached an image and the cad model.

I've been reading the manual,  and, yes I think doing one side at a time is the way to go - as the bottom edge is 'open' and it can't loft open and closed object (only one or the other). 

I'll also like to try the other way, just creating a very thin profile at the bottom - but the problem I see is that it's a curved profile (not sure if I can do this) - it appears that the version I have does not have the 'Bend' tool which is frustrating.

Thanks again
Tim

What accuracy are you aiming for?  A 3D intersection of two rotated tori has a similar cross section and gives a quick-n-dirty representation.

After a high level of accuracy - for a CNC machine to produce a prototype, then, if good, produce a mould from it (either using the prototype as a plug, mill two mould halves or mill two plug halves).

I should probably stop riding my boards up onto the beach ;-)

I've gone back to the books.  Just not able to create the shape I need to.

According to the manual, page 381, you can do lofting with guide lines - which, looks ideal - if it would work!

I've got an outline shape of the fin, which I have created 2 copies of - one trimmed so it represents the bottom edge of the fin, and the other trimmed so it represents the leading and trailing edges - these leading and trailing edges are what I'd planned to use as guides for lofting.

However, each time I try it, TurboCad pops up the following error:
"The resultant object of ACIS Solid type is selfintersecting or invalid.
The correct object can't be created."

I've attached the model.

Any suggestions?

Thanks very much
Tim

Just a minor rework:  wrapping a well-controlled loft through 90° to the tip with no intermediate profiles is a bridge too far.  I removed the coincident splines, scaled a copy of the penultimate profile and rocked it over 30°, locked the side profile off so it didn't confuse things and it lofted.

Hi Tim. Aside from Henry's and murray's advice I wish I could tell you why your lofting techniques are not working. Are you sure the guide lines are positioned sitting right? What about your workplanes? How are the profiles sitting? sometimes more is less with lofting with guidelines and profiles. The Fin below was created with two splines and two guidelines. The spline can be edited and the loft updates. Tcad takes into account for the side tapers and the guidelines do the front and back calculations. Good luck, and catch the Turbocad wave....

ps. I meant to say "sometimes less is more"

Just a minor rework:  wrapping a well-controlled loft through 90° to the tip with no intermediate profiles is a bridge too far.  I removed the coincident splines, scaled a copy of the penultimate profile and rocked it over 30°, locked the side profile off so it didn't confuse things and it lofted.

Wrong version? Wouldn't open in my v16, Murray.

Henry H

I've gone back to the books.  Just not able to create the shape I need to.

According to the manual, page 381, you can do lofting with guide lines - which, looks ideal - if it would work!

I've got an outline shape of the fin, which I have created 2 copies of - one trimmed so it represents the bottom edge of the fin, and the other trimmed so it represents the leading and trailing edges - these leading and trailing edges are what I'd planned to use as guides for lofting.

However, each time I try it, TurboCad pops up the following error:
"The resultant object of ACIS Solid type is selfintersecting or invalid.
The correct object can't be created."

I've attached the model.

Any suggestions?

Thanks very much
Tim

I see the same error message until I hide your outlines and disable "Use compound profile."

The attached screenshot and "KiteFinTest2MOD.tcw" show the result of lofting NOT using guidelines,  after adding one more copy of your lowermost profile at almost the very bottom, rescaling that copy to 1/10 size.

Henry H

It was V17, Henry.  Saved back to V16, now.

It was V17, Henry.  Saved back to V16, now.

Very nice, Murray.

Henry H

As is yours, Henry!  We skin some cats, don't we?

Hi Murray, I used the same method as Henry did on Tim's drawing and got the same results.  I think Henry's method of the splines layered then relocated and scaled is the way to go. Tcad does a fairly good job approximatiing  the outer edge, though lofting with guidelines can be a quick and easy way of sketching a design.The Pics below displays the differences in surface evaluation renders between yours and Tims. Can you explain why Tims original surface is not as consistent as your revised drawing? Can you achieve an even smoother surface? The third pic though not Tim's original design was created by lofting with guidelines,there is a noticeable difference in the surface eval.

My opinion is that Tim's drawing was inconsistent because there were coincident splines, so I took them out first.  The remaining stall point is the tip profile at 90° to the others.  I changed tack here, simply rotating the last profile and dropping it below z=0.   A good indicator of a poor surface is when it won't shell, but altering the last profile as described, it lofts and shells briskly, so I've done that, then sliced the shelled solid at z=0.  The part can still be adjusted by editing the profiles, jockeying the last one to make the tip conform more closely with the edge profiles, for example.  As this zebra plot shows, the tip is much smoother (this isn't trimmed).  

Thanks murray,That is nice. I agree Lofting without the guidelines does give more flexibility. I was just curious why Tim couldn't get the loft with guidelines to work. I got it to work though, using your revised drawing. I erased all the outer edges and lines then placed the workplane to world. Then adjusted the workplane origin to the end point on the trailing bezier. Then drew two 3d splines around the top and bottom outer edges (light blue). If you open the tcw file below just select the smallest bezier on the leading edge(finish select) then select the longest bezier on the trailing edge(finish select) then click on the guidlines icon and select the two light blue outer edge splines. Hit finish and  it works, though I think I could get the surface smoother if I added more foils (bezier) at the leading edge.

Hi guys

Thanks so much for your assistance here - really appreciated.

I've been reading about workplanes  -they certainly have caused me hours of frustration.  They sound straight forward when working with square boxes - but how they behave with compound curves and positioning objects in 3D makes no sense.

Murray - err... quite lost with several of your comments...    what are coincident splines?  Also, what do you mean by "won't shell" and "... then sliced the shelled solid at z=0" and what are you mean by "this isn't trimmed"?

I decided to use guidelines because, as Dean's noticed, when I viewed a quality render of the loft without guidelines the edges look jagged (eg straight lines instead of nice consistent curves).   And it looks like there are some inconsistencies with the surface - in the middle - some darker areas appear in the rendering - as Dean mentioned - less is definitely more with regards to lofting. 

Does anyone know why the snap-to-intersection is not very accurate?  When I resized the foil sections (the beziers) I used this to snap to the intersection of the outline and the construction lines - but when I zoomed in a lot, they were definitely not on the intersections - near but not exact - so I had to manually place them.

Is TC really capable of producing something that I would want to mill (particularly a mold!) - or am I using the wrong tool (ie I really need a near perfect model - smooth edges and surface - not a quick estimate of what the shape would look like)?

Thanks very much again  - really appreciate your assistance.
Tim

Does anyone know why the snap-to-intersection is not very accurate?  When I resized the foil sections (the beziers) I used this to snap to the intersection of the outline and the construction lines - but when I zoomed in a lot, they were definitely not on the intersections - near but not exact - so I had to manually place them.

Known bug. Intersection snap works OK with most 2D objects but not with curves.

Henry H

'Known bug."

  geesh now ya tell me.

Tim, Turbo cad should do the job for ya. Most likely you will need a stl file for prototyping. Tcad has built-in parameters for adjusting the precision of the surface. Look at the pics below. See the difference in the amount of facets. be careful with these settings cause you might freeze up tcad. The file size can get rather large. These acis settings are taken into account as well when you export the stl file. About the workplanes, yea, you really need to keep an eye on these. You can edit and save the workplanes. Also, there are parameters in the snaps options that influence their sensitivity. Remember when ortho is engaged it's a constant value. The angle options adjust the ortho step angle. When needing more precision joining entities it's probably best to have ortho off. 

What you see as jagged in render isn't actually jagged.  A curved surface gives an infinite number of possibilities for light reflection, so computer renditions limit them to a manageable number by fitting facets that approximate the surface, and that's what you see.  Workplanes aren't that complex.  You've drawn 2D splines, and they have to be on different planes to loft.  Each object in your drawing is associated with a coordinate system, and the x,y plane of that system is a workplane.  Select even a 3D curve and you see the origin and axes that it's associated with, transformations to the object are relative to those.  TC lets you put the origin anywhere, and orient its axes however you wish, so any translation and transformation of any object is possible relative to any point with any orientation.  That's quite a simple concept, yet almost infinitely flexible - when you understand how to use it with TC.
"Won't shell" refers to one of TC's capabilities.  When you loft open shapes, you create a zero-thickness surface.  When you loft closed figures, you create enclosed volumes.  You can "shell" either, which gives thickness to a surface, and makes volume solids hollow with constant-thickness walls.  That can't happen in all instances.  If a surface is too irregular or falls outside some other criteria, shelling fails.  Lofting is a pressure, or smoothness, distribution system, and lofting an open surface is less demanding than lofting a closed one.  The ability to shell is a good indicator of whether or not a surface is smooth.  You've oriented your fin flat on the world workplane, I've altered the orientation of the tip spline, so the resulting surface dips into the space below z=0, then sliced off the part that does so.  TC, like other CAD applications, adds and subtracts 3D objects from one another.  Slicing is a boolean operation that separates two parts of an object with a plane.
"Coincident splines" just means two or more splines occupying the same space. 
TC is capable of making your fins in many more ways than one, but its capability has a learning curve.  It can't create the objects you want it to unless you know how to tell it to.

Thanks guys. 

And thanks Murray for the explanations..  it's starting to sink in.  Can you suggest any other ways (of creating these types of fins) I can look into and learn?  ie, is there a better way (less fiddly and yielding a smooth surface)?

Dean I'll try what you recommend but based on what Murray says, it sounds like I shouldn't need to.  So when I get a surface that looks good enough, I'll export the stl and mill it.

Thanks again
Tim

Tim, you're doing pretty much everything right except for the tip.  Your original file, once I'd taken out the duplicate splines, lofted through everything except the last profile, so I placed a copy of your last vertical profile so it guides the loft below the workplane.  The aspect ratio of the last profile is changed, because you need a taper to the tip.  The loft is smooth enough to shell 2mm thick, some of which drops below the workplane.  Then I envelope the object in a box that's sitting on the workplane and intersect the two, after which the fin is a solid with a flat centreline.  Have a look at this file rendered.  You'll see the tip of the surface loft protruding below the box in the first copy, the thickness that protrudes below when the fin is shelled, and lastly the shelled fin after it's been intersected with the box.  The perimeter of the loft doesn't exactly match your guide splines, up to .2mm variation, but I'm confident that it's as smooth as you'd want.

Thanks very much Murray.  I'll try reproduce it from scratch myself, then will mill it.

Out of interest, how did you find/notice the duplicate splines?

Regards
Tim

Out of interest, how did you find/notice the duplicate splines?

Clicking to select what looks like one spline brings up the ambiguity selection list.  Selecting one of the choices and deleting leaves the duplicate.

Are there any alternatives for creating a compound curve solid with TurboCad - eg one of the fins mentioned above - to a specific outline curve and foil profile (not just a 'near enough' result)?

Really not happy with results to date (models, error messages, the unintuitive work-around's required, and the time it takes to produce something relatively accurate).

Thanks
Tim

Are there any alternatives for creating a compound curve solid with TurboCad - eg one of the fins mentioned above - to a specific outline curve and foil profile (not just a 'near enough' result)?

Really not happy with results to date (models, error messages, the unintuitive work-around's required, and the time it takes to produce something relatively accurate).

Thanks
Tim

Since everything we build, and everything a piece of software produces, is either near enough or not near enough -- is 0.00001" close enough for this particular object? I copy-and-pasted your Outline_sides, your OutlineCurve_bottom, and just the topmost foil into a new drawing; moved the latter 0.00001" in the Z direction; and lofted the outlines to the foil. Applied Format>Create Solid>From Surface to the result. Drawing is attached.

Henry H

THUFFMAN,

How did you go with this project as I am trying to form something with different curved surfaces for a mould and have been following this thread closely.

thanks
exdraftee