Needing help drawing fan blades using loft tool with rails

[mgianzero]

I'm a newbie to mechanical CAD work, never mind Fusion 360.  I'm attempting to make a fan with complicated blades - they are twisted in many directions with a distinct profile on each edge.  I've gotten the general blade bend I wish, but now I'm struggling to trim the leading and trailing edges of the blades using a specific profile I want.  

Ideally, I was hoping to using the loft tool to not only define the basic shape of my blades, but to also define my leading and trailing blade edges with no success. I attempted to do the trailing edge using a revolving cut and leading edge with a fillet.  Not exactly what I want, not to mention, seems more complicated than it needs to be.   How would I do this?

I've attached a pic of my fan as well as the Fusion 360 file to show my problem.

Any help is very much appreciated.  Thanks everyone!

Marc

[davebYYPCU · Accepted solution]

The tip of the rib is not touching the trailing edge rail.

This is the reason I redraw the tip rib in my file.

The Rails need to exit first, 

When making the tip rib, you need to Project > Intersect each rail, into the tip rib sketch, first thing to do, 

Then hide the rail sketches. 

Now the tip rib has two purple points. 

Your rib Has to snap to these two points or Loft fails every time.

You will get there, no panic, I was talking about Project > Intersect, early in the thread, and probably forgot to highlight that in the screencast...

[mgianzero]

So I see.  Thanks again Dave.  I should have realized that.

So it looks as though you get into a dilemma trying to find out whether to determine your rails or your profiles first.

Here's yet another attempt at drawing the blades, but I don't think that using sweep will ever get me what I want as you can see here.  But I just don't know what my next step would be to determine the trailing blade edge.  By the way, my airfoil profiles look horrific, but I'm not really focusing on that detail at this time.  Mostly just the leading and trailing edges.

I am just going around in circles here?  I don't want to waste anybody's time, but I want to be able to fully understand my 3D drawings and recreate them accurately.

Marc

[davebYYPCU]

Gooday Marc

So with this new file,  I agree about the rib profiles, and like me,

You are finding that this project is not a beginner project.

I totally agree with you about the Sweep, not being right for this project, 

I am sending you a private message to give more detail answers. 

When you open this forum, the message section in black will have a number next to it,

click on Message to open them.

This file is still in setting up stage, you have the two ribs, and leading edge curve, made a loft from those 3, all OK.

You have top and front curves for the Trailing edge, Next

Create new Sketch, select any plane, because this sketch will be a 3d sketch and any random plane still works.

Hide both ribs, 

Project >Intersection Curve, select top trailing edge curve

Select front trailing edge curve, click OK.

Because your ribs won't line up with this new trailing edge,

cart before the horse stuff here, 

we make new rib sketches, and hide the old ones, just like my file.

Check for my PM.

[mgianzero]

Well, I ended up redoing my drawing once again (this time even neater) using an airfoil around a 2-dimensional profile and I can draw the full blade using Patch Mode and selecting each spline as my base and tip profiles (not really a profile but just a line edge) and I can draw the blade using Loft using my 2 rails from leading and trailing edges - remind you this is Patch Mode only.  But I cannot loft using Model Mode as I still get that "the loft would intersect itself" error.  I don't know if I'm making my airfoil profile too small or what.

Attached is my file for all who wants to look. davebYYPCU is without Fusion 360 capabilities for the next 10 days, so I thought I'd continue the conversation here to see why I get this "new" error with Loft.

[laughingcreek]

When you un-suppress the loft, you can see it crinkles in the middle region.  when your lofting the whole thing, this cause the top and bottom to touch or cross, and fussion doesn't care for that.  one possible solution is to put in another cross section in the middle

[laughingcreek]

I think it might just be easier to just drop back to the idea of using a sweep.  Here's your file back, just added the one feature.

[laughingcreek]

I meant add a third rail.  much easier than another cross section

looking at your rails I see that they connect to the centerline of your foil shape, but not to the edge of the foil.

[laughingcreek · Accepted solution]

And here's your file back with a loft.  Changes made where to put the foil profiles coincident with the center lines all the way around, and eyeballed 2 more rails about mid section.

[mgianzero]

Alex,

This is great news!   I've been banging my head with the snag for the last few days and now I think I see what you have noted.  

I think I'm saying this right when you pointed out that there are "crinkles in my airfoil" which can make a loft model overlap and therefore crash - so this is what is meant by dreaded "the loft would intersect itself" error.  I never fully understood that problem despite all my reading on the community forum which sort-of explained that.

So, knowing this, what is a good technique to analyze for intersecting shapes in the future?  I applied two inspection techniques, curvature map analysis and zebra analysis, to this same blade and it seems to pick up a crinkle in my airfoil.  Is this what you suggest?  Because I have never used this options before and was thinking this is a good application for this.  If so, which one is more appropriate for my purposes? 

Below are my two analysis of this same blade that I designed.

Thanks again Alex!

Marc

[laughingcreek]

To be honest, I've never used the analysis tools to examine if a loft will work.  An interesting idea  that I'll have to give some thought to.

I do use those tool all the time to examine the quality of surfaces of course.  Very useful tools to have, and I'll use them to make a loft better.  Mostly use zebra, but they all have a use.

The analysis tool that may be the most useful is curvature combs in the sketch environment.  Every thing starts with a curve.  You have to have clean curves to get clean surfaces!

By now you've worked your way down to the file I posted in post 28.  That's going to be the general approach towards fixing things like this.  The more geometry you have, the more control you get over the shape, at the expense of having more places to make a mistake (of course).

[mgianzero]

So, I've mostly resolved my issues with the lofted airfoil-shaped blade with everyone's help.  So I'm not sure if I should continue here with additional questions or not, but it's the same project and probably a simple answer.

I've continued with the project to draw out more details in the hub using "revolve" but I can't seem to get rid of this "pie slices" that show on to top of my hub as I revolve it 15 degrees in each direction with two different profiles.  How do I remove them?

Please let me know the etiquette of using this forum if this should require a new topic and close out the old thread or not.

Thanks everyone!

Marc

[laughingcreek · Accepted solution]

There are advantages to keeping an old thread going, and to starting a new one.  Either way, as long as everybody is being civil it doesn't matter which way you go.  People following this thread will pick up on your questions faster, and not point out all the things that have already been pointed out again and again.  On the other hand, if your not getting an answer, or you want to throw it to a larger audience, you can start a new thread.

Your foil doesn't quite fully intersect with the hub on the leading edge.  see pic below.  The original blade also never go combined with the whole thing, you can see that in the screen cast.

That gets fixed with a combine command.

The pies get fixed by revolving the full 360 all in one shot

the fan blades are patterned by their faces.

Voila!

[mgianzero]

Alex,

Okay, I will keep that in mind regarding posting in threads - as long as we are all learning and following the same project, I'll just keep posting.  Hopefully I'm reaching near the end of this project and it has been quite a learning experience as this one was tough part to draw - especially for a beginner like me!

However, I think some of your suggestions here are not working for me. 

Regarding eliminating the gap between the blade and the hub, actually the gap is much bigger but I did a trick that Dave did which was to draw the blade a bit inside the hub to mostly cover this gap from a plane resting on a curved surface - but if I really kept the blade where I want it to be, the gaps would be much bigger on both sides as seen in my first pic.  (That's because I moved my blade base plane in from the true 82.5 mm to 79.5 mm.)  I'd really prefer to keep blade out more so I don't have to fudge a distance for the blades.  And when I did your combine command on these two bodies, nothing really happened.  It just made both bodies one body, but gap remained the same.  Unless I'm misunderstanding your purpose of suggesting it here.

Second, the whole purpose for my 15 degree pie cuts is because of the profile which is drawn on the underside.  Making it 360 degrees eliminated this ribbed effect.  (See second pic below).

Lastly, the reason I did a split body cut on the ends of my blade with a circle was to trim all the blades to make them rounded as you can see in my model.  Didn't know of another way to do this since trimming it with my radial profiles doesn't fully cut the ends through the same 30 degrees as the underside design.  Hard to explain I know.

Marc

[laughingcreek · Accepted solution]

OK, here's another screen cast.

you'll note the surface of the blade is still a little funky.  This can be solved with a rail along the middle probably.  or just leave it the way it is.

The purpose of combining the blade to the hub was, indeed, to just have one body. 

But now that it's combined, you can select that little face and just delete it, and the model heals itself.  This is a bit of a cheat, but it works here.  Typically you would build the blade longer  on each end and trim to length.

I total missed the ribs. (turn it over Alex!).  That can still be dealt with in a similar manor. full revolve to cut things out.  15 degree join to add the rib back in  (I created a new body the first time on this revolve, had to go back and change it to join). 

add the rib to the pattern command for the blade..

I don't see the split body in your model to trim the fan ends, but that sounds like a fine way to do it.  but now that we're doing a full revolve cut, you can also adjust sketch "Hub Profile #1" as needed to do it.

[mgianzero]

Alex,

Once again, I think I've learned about 10 things with just your reply!

First off, I didn't realize that when you click with your mouse wheel it moves your pivot point --  (duh - again a newbie just learning Fusion).

I really like the idea, although you say it's cheating, of deleting the faces adjacent to each other in a combined body so that it mends itself -- really cool!

I also see your point of just revolving a full profile for the hub and then adding back the rib - yet another neat trick.  I still don't understand why Fusion inserted these pie lines everywhere I partially revolved my profile.  Seems that if you spin it in increments, it will still give you a smooth, one piece body.

I noticed your zebra technique for finding the wrinkle in my blade design.  Any ideas on how to smooth this out a bit?  Because my actual fan part is very smooth in reality.

Marc

[laughingcreek · Accepted solution]

Ok, so it's not necessary "Cheating" to delete little faces like that.  It does the job.  It IS good design practice to make every attempt to avoid creating these things in the first place.  They have a way of creeping in and breaking a perfectly parametric design.  And every now and then you might find that it doesn't work, right when you were REALLY hoping it would.

Here's a screen cast of adding a mid rail to smooth that face out some.  (post 28 has a file with the same thing.)

[mgianzero]

Okay Fusion 360 community,

After playing around with this fan project for weeks, being the newbie that I am, I think I'm finally reaching the finish line!  But before I celebrate, I wanted to share my latest drawing with you all to tell me what you think - please feel free to give me feedback, particularly on ways to make my drawing a bit simpler and more streamlined.

Here are a few things I either have questions about or would be nice to cleanup:

1) The only "convenient" way I found of drawing this curved-blade tipped fan is to draw each edge on a plane and lofting it.  (This is something that Dave (DaveYYPCU) and Alex (laughingcreek) spent a great deal of time with me perfecting my technique - thanks guys!)  Since these fan blades are curved on the end, I had to cut them (I used split body with a circular shroud) and "welded" (not sure the word to use here) the base of the blade to the rounded center hub by simply deleting the exposed faces.  However, I wasn't sure how to position these blades in relation to the hub.  Should the midpoint of the plane for the profile blade base lie tangent to the hub?  Then what about the tip of the blade?  Do I make the plane for the profile of the blade tip parallel to the blade base or tangent to the shroud?  Remember, the base and tip of the blade are offset from each other a bit.  Hope I'm making sense here.

2)  So I know that most of my drawing is completed to fairly represent my current fan blade, but how do I best tweak the fan profiles (airfoil shape as well as rotation) in order to make a different blade shape?  Right now, in order for me to change my leading and trailing blade edges, I edit my "top view" sketch to whatever profile I want.  Then the other "rails" should automatically change to match this new layout since they are projected to other planes.  In order to change my airfoil profiles, I edit the sketches for my base blade and tip profiles to my liking and then I move all my points around on two airfoils that correspond to each side to make it match.  Seems kinda cumbersome to do it this way.  Is there an easier way?  

Thanks in advance for any additional comments or suggestions.

Attached is a picture of the fan blades w/ hub along with the F360 file.

Marc

[mgianzero]

After taking some time to investigate topic #1 above, I think I've been able to determine that my blade tip, although the profile seems fairly accurate, it needs to be moved counterclockwise (more twisted away from the blade base) by about 15mm.  So what's an easy way to do this?  I've been trying to use the "Copy / Move" command by things just get messed up when I try to just move sketches on that plane.

Ideas?

[laughingcreek]

did you work this out?

It looks to me like the process of rotating may be a little tedious. start by rolling your time line back to the "blade base profile " sketch.  select every thing on that sketch and "move" to rotate and reposition.  things are going to break in the timeline, so instead of immediately going back to the end of the time line, step forward one step at a time, and fix things as you go.

The work flow you guys worked out is admittedly a little strange to me, so it's a little hard for me to follow.  I understand the chicken and egg problem you where trying to avoid,  but it seems maybe you were over thinking things a bit in terms of the order you created the profiles and edges.  This is contributing to the difficulty your having now in making adjustments

[mgianzero]

Alex,

Well I tried your suggestion "select every thing on that sketch and "move" to rotate and reposition" but it doesn't seem to want to move at all - strange.  What am I doing wrong now?

Also, if you think my workflow is strange, please feel free to make suggestions.  I'm still new to all of this and don't want to create bad habits.

I will say a few things to support my workflow ...

1)  I drew a majority of the hub using a revolving profile at the beginning because I found it was much easier to picture where my blades would go this way.

2)  The next thing was to design the blades.  Here I used a simple curve to place the base and tip profiles using a simple curve and initially projected it in 3D as a two-dimensional blade (no airfoil) just using Patch Mode and lofting with two rails.  I used various plane views and used "Project - Include 3D Geometry" to create the rails in 3D space.  Perhaps this area is where it gets a little messy, so I'm open for suggestions to improve it.

3)  Then I did various cleanup edits to make the blades "weld" to the hub, cut the blades to a curvilinear outside edge, and I cut out the "ribs, holes and made fillets" which I revolved into the bottom of hub.  Since this used "cut" instead of "join" I made another new profile to do this.

4)  Lastly, I ended up finishing up the "center snout" of the hub because I didn't know another way to make the bolt pattern any other way.  I actually had to recut the center hole to clean out the bolt sleeve protrusions into the center hole.  That also seemed a little clumsy but didn't know another way.  I could have done this at the beginning, but didn't think about it until later.

Feel free to critique and keep up the good suggestions.  Hoping someday to become a worthy Fusion 360 expert who can support others on this forum!

Marc