FreeCAD: A moderately complex example

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awake

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Actually, that title may be claiming too much. What I should say is, this is one of the more complex things that I have modeled in FreeCAD. The complexity here is not in terms of quantity of parts - any of the engines I have modeled have far more - but rather in the techniques that were needed, especially to produce the 3d sweep path for the impeller. Also challenging were the sweeps with the ever-increasing radii. These parts were designed for 3d printing (FDM), so the design had to take that into account.

Not as complex or challenging, but new to me, was designing the motor mount to be laser-cut from mdf.

I've attached the models and also pictures of the results. It uses the blower motor from a discarded over-the-stove microwave. Does it work? Oh, yeah! It is noisy (whines), but produces a lot of air. Now I need to figure out how to quantify the output ...
 

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Nice CAD/Printing work. Those kind of projects are fun to model up! It's funny how complicated it appears when 3D modeling something like this. I went through a tutorial (For Pro-E) on modeling an impeller many years ago that went ("Simply") something like this:

1. Extrude the circular base.
2. Extrude a curvy shaped vane on top of the face of the disk (Viewed "looking down on the circular face").
3. Pattern those extruded vanes.
4. Create a "Revolved cut" (Viewed as a "side view") & sweep the cut about the (already) created centerline.
5. Add the fillets as desired.

I was pretty tickled when it all worked, & looked like quite the complicated bit of modeling when I was done. Of course the housing is another fun exercise. :)

Disclaimer: It's not my intention to tell you or anyone else how to create 3D models in your favorite flavor of software, or distract this thread.

Just sayin'

Nice work Awake!

John
 
Similar work flow, but not exactly the same. The base is as you say, a simple circular extrusion. For the vanes, I created a 3d extrusion path by creating and intersecting two "surfaces." One surface reflects the simple radius as one looks down on the impeller from the top; the other reflects the "ogee" shape of the blade as it sweeps up from the center to the outer edges. I "sweep" (or extrude) the basic blade profile along this 3d path, then cut off the excess bits left over. Hard to explain in words ...
 
Nice work! I happened to be looking at impellers today for modeling practice and read your post this afternoon.
Too often FREECAD is underestimated. If you can model like this in FreeCAD, you can succeed anywhere else.
How did you set up your guide curves to get it to solve?
 
Actually, that title may be claiming too much. What I should say is, this is one of the more complex things that I have modeled in FreeCAD. The complexity here is not in terms of quantity of parts - any of the engines I have modeled have far more - but rather in the techniques that were needed, especially to produce the 3d sweep path for the impeller. Also challenging were the sweeps with the ever-increasing radii. These parts were designed for 3d printing (FDM), so the design had to take that into account.

Not as complex or challenging, but new to me, was designing the motor mount to be laser-cut from mdf.

I've attached the models and also pictures of the results. It uses the blower motor from a discarded over-the-stove microwave. Does it work? Oh, yeah! It is noisy (whines), but produces a lot of air. Now I need to figure out how to quantify the output ...
What are you using that on?
 
Nice work! I happened to be looking at impellers today for modeling practice and read your post this afternoon.
Too often FREECAD is underestimated. If you can model like this in FreeCAD, you can succeed anywhere else.
How did you set up your guide curves to get it to solve?

Thanks, Zeb. Rather than trying to describe this in words, I thought it would be easier to make a quick video. Well ... it didn't turn out all that quick, and it definitely is not polished or smooth, but hopefully this will answer the question:

YouTube is "processing" it now, so it may not be available for another 30 minutes or so. I'll be glad to answer any questions.
 
What are you using that on?
Hi Richard,

It remains to be seen whether I use it or not! I made it to be an assist for the smoke extraction on my new-ish K40 laser cutter. The built in fan, along with the tiny opening, does not do a great job of extracting the smoke. I 3d printed some adapters to use with my electric leaf blower, and that definitely helps, but it is a bulky and awkward setup. If this will do the job, I can mount it under the shelf where the K40 resides and have it permanently hooked up. I still have to print the adapters to hook everything together, so I don't know yet whether all of my efforts to make this impeller have been in vain. No, scratch that - I enjoyed the journey of learning how to achieve the design, so even if I wind up not using it, it will still have been a fun and worthwhile project!
 
This was excellent thank you. Your narration was also very good. I followed along using Plasticity (Parasolid), which for fillets is akin to cheating.
FreeCAD sure could use a menu to attach your sketch orientations using existing geo, but it was great to see how you aligned the transformations exactly. Any misalignment would cause the feature to fail and many of us would have quit. Also nice that you have everything parametrized on a spreadsheet.

In my case I cut the spun profile as you did, added a thicken command normal to the surface, and filleted the rest. Knowing how to surface a complex fillet manually is the true skill to have as even the fancy toys may not produce the desired effect.

ImpellerTutorial.png
 

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It seems you were able to totally over complicate this. Although you may have your reasons,,

See my explanation above (Post #3) & try it.

It's cool how you use the spread sheet to drive your model, but unless you're doing multiple variations of this, I don't understand why you would do this.

I also don't understand why you created the vanes as these fancy swept surface features (Or whatever you call them in your CAD...), they can be created as I mentioned above, & use a revolved cut to trim to the shape desired.

In my example as I explained above, there are no fancy sweeps, surfacing, or using trajectories to define all these crazy "Guide curves" as you mention. Just straight up solid modeling.

Am I missing something???

John
 
Actually, that title may be claiming too much. What I should say is, this is one of the more complex things that I have modeled in FreeCAD. The complexity here is not in terms of quantity of parts - any of the engines I have modeled have far more - but rather in the techniques that were needed, especially to produce the 3d sweep path for the impeller. Also challenging were the sweeps with the ever-increasing radii. These parts were designed for 3d printing (FDM), so the design had to take that into account.

Not as complex or challenging, but new to me, was designing the motor mount to be laser-cut from mdf.

I've attached the models and also pictures of the results. It uses the blower motor from a discarded over-the-stove microwave. Does it work? Oh, yeah! It is noisy (whines), but produces a lot of air. Now I need to figure out how to quantify the output ...


Thank you for showing that FreeCAD can actually be made to work (I haven't succeeded to date - - - although I've been hesitating at trying again for a while - - - I just found some things too frustrating!!!)

Looking at your vane design - - - - I have been looking at centrifugal blower design for a while - - - I'm looking at something in the 12 to 20 kW size range and find that most of the stuff for sale is using reverse curved vanes, your is using forward curved vanes.

Would you care to share as to your design thinking re: this particular section?

TIA
 
I also don't understand why you created the vanes as these fancy swept surface features (Or whatever you call them in your CAD...), they can be created as I mentioned above, & use a revolved cut to trim to the shape desired.

As he showed in the video, Freecad fillets are very brittle and tend to break with complex objects when edges meet at odd angles. This was a way around that.

Freecad uses a 3rd party 3D kernel, Open CASCADE Technology (OCCT), so sometimes it's difficult for the developers to fix or work around long standing issues like this.

In my example as I explained above, there are no fancy sweeps, surfacing, or using trajectories to define all these crazy "Guide curves" as you mention. Just straight up solid modeling.

Am I missing something???

Luckily for you (and everyone), Freecad is completely free to install (PC, Mac & Linux) and use. Try out your method and report back on how it worked.
 
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It seems you were able to totally over complicate this. Although you may have your reasons,,

See my explanation above (Post #3) & try it.

It's cool how you use the spread sheet to drive your model, but unless you're doing multiple variations of this, I don't understand why you would do this.

I also don't understand why you created the vanes as these fancy swept surface features (Or whatever you call them in your CAD...), they can be created as I mentioned above, & use a revolved cut to trim to the shape desired.

In my example as I explained above, there are no fancy sweeps, surfacing, or using trajectories to define all these crazy "Guide curves" as you mention. Just straight up solid modeling.

Am I missing something???

John

Hi John,

Thanks for the comment. A couple of responses:

On the spreadsheet, you have put your finger on the reason - this was a matter of testing different designs and trying out different parameters. I "only" printed the case twice and the impeller three times, but there were several intermediate stages where I tweaked the design and looked to see how the parts would interact. Over time, I have found it worthwhile to generate a table of parameters for anything more than a very simple one-off. At this point, this project as a whole is likely to be a one-off, but it was not simple, so it was very helpful to have the parameters organized and available. I should add that I have had the experience of designing a one-off that later turned out to be the perfect foundation for a new variant. Whenever that has happened in the past, it sure is annoying if I have to go back into each and every sketch to update a parameter, and conversely it is so nice when I have all the parameters broken out like this and can change everything at once.

On the complexity factor vs. a more simple approach - absolutely I could have taken the simpler approach, and in fact, I did just that for the first impeller I modeled and printed. A simple sweep along a 2d curve gave me the vanes at full height; then a simple revolve cut them into the desired shape ... sort of. Note that with the simple approach, the "ogee" curve of the impellers comes out skewed with respect to the cross section of the blade. Does this matter? Probably not; given that this is being 3d printed on a so-so FDM printer, I'm guessing the variations from one print to another would have as much effect on efficiency as the difference between one approach or the other.

But I wanted to challenge myself to produce a blade that followed a smooth, continuous sweep, in part as a way to learn more about how to make more complex shapes. There are situations where one needs, say, a pipe to follow a curve that cannot be defined only in a single plane - e.g., a fancy exhaust header. Another factor was wanting to fillet the edges of the blade, and as Krypto notes, FreeCAD doesn't always succeed with fillets, especially for shapes that have undergone several steps like this. This is, of course, a limitation of the tool ... but all tools have limits, and I like to discover ways to achieve results in spite of the limits.

Bottom line: I wouldn't say that you are missing anything; I just made different choices based on what I wanted for the final outcome and how I wanted to be able to make changes to the model. I make ZERO claims that I have done this the right way, none at all. I only wanted to share my "work in progress" in learning how to model things in FreeCAD, knowing that 1) there are other tools that other users will prefer, 2) there are other approaches that others will prefer, 3) there are other people who could have done all of this much better whether in FreeCAD or in any other software!
 
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Thank you for showing that FreeCAD can actually be made to work (I haven't succeeded to date - - - although I've been hesitating at trying again for a while - - - I just found some things too frustrating!!!)

Looking at your vane design - - - - I have been looking at centrifugal blower design for a while - - - I'm looking at something in the 12 to 20 kW size range and find that most of the stuff for sale is using reverse curved vanes, your is using forward curved vanes.

Would you care to share as to your design thinking re: this particular section?

TIA

Hi Joe,

I know you have not had a happy experience with FreeCAD, and as I acknowledge in the video, there are definite limits and annoyances to the software. I have to say that it took a while before I fully committed to FreeCAD - I dabbled with it from time to time, and every time it felt like I had to climb a mountainous learning curve all over again. At that point I was designing in 2d CAD, then attempting to generate the 3d model in FreeCAD. I'm not sure at what point I finally "tipped over the edge"; at some point my thinking finally shifted over to the 3d approach (at least FreeCAD's version of it). Then for a while I would generate the model in FreeCAD, but go back to my 2d CAD program to draw up the plans. Nowadays, I do all my design in FreeCAD, and use FreeCAD to generate the plans, so I rarely ever use my 2d software for anything.

Honestly, I don't know enough about impellers to be sure what you mean by "reverse curved" vs. "forward curved" vanes. I'm thinking the difference is dependent on the direction (clockwise or ccw) that it spins? FWIW, I followed the design of other impellers I could find - the electric leaf blower for one, and pictures of various impellers on-line. The impeller shown spins clockwise (which is probably obvious from the housing) so that the outer edge of the vane tips back from the direction of rotation. If it were the other way, I would think the blade would tend to "scoop" air inward rather than pushing it outward. But did I mention that I don't know enough about impellers to be sure what I am doing? :)
 
Hi Joe,
snip

Honestly, I don't know enough about impellers to be sure what you mean by "reverse curved" vs. "forward curved" vanes. I'm thinking the difference is dependent on the direction (clockwise or ccw) that it spins? FWIW, I followed the design of other impellers I could find - the electric leaf blower for one, and pictures of various impellers on-line. The impeller shown spins clockwise (which is probably obvious from the housing) so that the outer edge of the vane tips back from the direction of rotation. If it were the other way, I would think the blade would tend to "scoop" air inward rather than pushing it outward. But did I mention that I don't know enough about impellers to be sure what I am doing? :)
https://www.cincinnatifan.com/centrifugal-hdbi.htm
for an example of the backward inclined blower - - - - aiui you actually get higher efficiency with high air volumes - - - - that is from reading not experimenting!

Was able to find a page that has the three types (that I know of) on it - - - there is some reasoning as to which to choose on the page

Centrifugal Fan : Backward Inclined Blowers: Cincinnati Fan


I may just try a personal message to you when I have some time available in my attempt to learn FreeCAD (there is no way a stupidly designed tool is going to beat me!!!!!!!!!!!! - - - - I've had to learn to use far too many other such and I'll get this one one way or the other!!!!) .
 
If I have understood what I am seeing, my design uses the backward inclined approach. That's a big "if" ... !

Sure, PM me. I make no claims to expertise, but I can share what I have learned!
 
It seems you were able to totally over complicate this. Although you may have your reasons,,

See my explanation above (Post #3) & try it.

It's cool how you use the spread sheet to drive your model, but unless you're doing multiple variations of this, I don't understand why you would do this.

I also don't understand why you created the vanes as these fancy swept surface features (Or whatever you call them in your CAD...), they can be created as I mentioned above, & use a revolved cut to trim to the shape desired.

In my example as I explained above, there are no fancy sweeps, surfacing, or using trajectories to define all these crazy "Guide curves" as you mention. Just straight up solid modeling.

Am I missing something???

John
I think his post has more to do with the process and as Krypto mentioned, stabilizing a very difficult modeling kernel to run smoothly on a spreadsheet. In the video he explains that FreeCAD is unable to handle complex overlapping fillets. The solution he presented can be applied to more difficult problems.
I think the one advantage his solution has to extruding from the top is that the thickening geo is normal to the surface of the vane, not extruded along a flat vector. I used the thicken command in my case, but this would have failed later in FreeCAD because of the fillet solver's limitations.

This is an example where Parasolid did a beautiful job joining the wing and fuselage in one click. The problem is that the transition would be aerodynamically dirty on my little RC. I could use an approach similar to that described to better control the transition at the trailing edge.
drag.png
 
Thanks Andy (& others) for your comments.

It seems a shame to have to work around limitations of the software to accomplish things, but I haven't worked on any software where I DIDN'T have to do that. I also understand now why you did the spreadsheet/parameter thing, I've been bitten (Like many of you..) in creating just a "Quick & dirty" design (just to get 'er done) & then having to go back to that design & seeing how sloppily I modeled it, taking as much time fixing my mistakes as creating a new model.

Fillets are a pain, especially depending on where they are in the model tree (order of operations), such as drafts..

CAD is a fun tool to play with, & there is nothing wrong with your methods. I often explored many different methods to create features in my CAD models just to see if it "would work".

"Try out your method and report back on how it worked." : Krypto: I did just that in post #3).

Keep up the modeling, it all looks good. In the end, the final result is all that matters, & when you're holding the part in your hand, it doesn't matter how you got there. It's kind of the opposite of "Enjoying the journey" & really just enjoying getting to your destination.

Nice work Awake, keep it coming.

John
Last edited: Today at 8:47 AM
 

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