Post SOLIDWORKS Designs Here

[lathropdad]

Bill,

Have you used the simulation function to do a stress analysis of your fuselage? I made a change to my BearHawk 4 place and modeled that change to check my choices for tubing sizes.

I have done stress studies on tube structures I do for the race cars I build. And I have done torsion tests on the completed race cars. There is an excellent correlation between what I model and what I find in actual testing.

In another post, there is a description of how to make flat paper templates of the tubes in the cut list. it is a very useful capability/tool. Wish I had learned it years ago.

I looked doing a stress analysis for my fuselage as an educational exercise and quickly decided that I had no clue as how to model the loadings or what they would be like. I have only done the stress analysis on one part that had failed on another's builder's project and another part where the loads were very simple to know and calculate. The analysis I do on my race car frames is to develop a single number that I can then check on an assembled car and I use that number in calculating setups for the cars. By comparison a race car is a very simple system to analyze.

[cwilliamrose]

No, I haven't played with simulation to see what I could learn for a few reasons. First, since the tubes are separate bodies I wouldn't think the tool would accept the fuselage structure -- I only have the light version available. And then there's the questions of what loads to apply. I'm not a structures guy so I would likely get answers to questions improperly asked. One more issue is the fittings attached to the fuselage where the loads should be applied, That would again require more than Simulation Light since you would be dealing with an assembly once the fittings became part of the structure.

[SFahrner]

As a retired (?) aeronautical engineer/stress analyst guy who still does occasional consulting work using the SW/Simulation Advanced Professional package, I give a tip of my hat to cwilliamrose for his comment:

“And then there’s the question of what loads to apply. I'm not a structures guy so I would likely get answers to questions improperly asked.”

Many times in dealing with clients, the biggest problem in creating a useful FEA model is the lack of knowledge about the real loads (especially dynamic loads) to which the part/assembly will be subjected. It turns out that an analytical model that is “accurate” to within 5% isn’t very useful as a failure predicting tool if the applied loads aren’t known within a factor or 2 or 3…

Given that we are usually dealing with loads that aren’t well defined, I think the most useful application of the Simulation package in SolidWorks is for “Qualitative comparisons of design changes, rather than quantitative predictions of failure conditions”.

Dispensing with the analyst’s vocabulary, this means using the analysis tools to simply compare stresses for different shapes. For example, use the Simulation Tool to determine the stresses for a bracket with any convenient load (I often use 100lbs). Then modify the bracket (add a lightening hole, change a fillet radius, etc.) and compare the stresses in the “new” bracket to the original stresses. If the stresses are lower, you have likely improved the design…

The weight of the part(s) is available with a click on the “Mass Properties” button, so you can also readily compare the weights…

Also, regarding paper patterns for mitered tubes:
I still use the following elegant piece of shareware written years ago by Giles Puckett:

http://rorty.net/news/tube-miter-program-giles-puckett

Even though I’m fairly fluent in SolidWorks, I find Mr. Puckett’s excellent program to be quicker for most of my applications…

[Mark Meredith]

Hi Mark,

In a part window try Insert > Curve > Curve through XYZ Points...
You will be asked for a "Curve File", Browse for your Notepad text file and press enter.
Note that SW by default looks for a .dat file, not .txt - but when you browse for it you can change the browsing window to look for .txt file types.
Note also that the .txt file should be formatted in the form of a single line containing the delimited X,Y, & Z coordinates for each point (no headers or any other text).
The result will be a curve feature in the history tree (probably a good idea to rename the feature with the name of the airfoil).
In any sketch you can now Convert that feature into a black (fully constrained) sketch entity. By deleting the "conversion" constraint (thus making the entity unconstrained - blue) you can now do some cute manipulations. For example, in the sketch draw a straight construction line with a length equal to your required chord length and angled at your required angle of attack, and then drag the blue airfoil end points to the construction line end points. You now have your airfoil scaled and correctly oriented.

Hope this helps

Jeff,
That was easy! It took minutes to convert my airfoil, then set the chord and incidence. Way easier than what I did before on my Chipmunk, which was to import a sketch drawing, size it, set the angle, then draw a spline on it. Thanks! Mark

[Mark Meredith]

Jeff, Bill,
As an experiment I tried the above using the airfoil (saved as a part file) brought into a new part file. Worked fine. I could build separate parts around the airfoil.

I also built a practice part from a textbook (a bench vice) with a base and multiple movable parts added to it. This method started with a top down assembly. Open a new assy, insert a new part (the base) and draw it. Then insert a second new part (the slide), using Offset Entities to set the relations between the parts (in this case, a .010 space around a slide). When finished it would not move. So I deleted the coincident mates and built new mates so the jaw could slide. That seems like a fairly good way to work...only real difference I see it that the top level is an assembly instead of a part.

I'll give this a whirl building my tailwheel as full tree of parts starting from the tailwheel assembly. Then will mate the assembly to the fuselage. Thanks!

[Mark Meredith]

Sorry about the images. For some reason you insert the images into the body of the message and they appear again at the bottom of the post. I deleted those 'extra' images and it seemed to be OK at work. Now that I'm home the images are gone. I have no idea what the problem is... I'll get the photos back into the message tomorrow.

Bill, the images all showed upon my computer fine.

[cwilliamrose]

Thanks Mark, I replaced them this morning and they seem to be OK now.

[Mark Meredith]

VR3 uses the tubes as individual models to machine the fishmouths on their CNC equipment. When you receive a kit from them the parts fit together like a jig saw puzzle. If you're building a fuselage from scratch you likely won't have access to the machinery VR3 has so models of the individual parts would have little or no value.

Within the past couple of months there was an article in Experimenter in Sport Aviation, by Brian Carpenter. He described using SolidWorks to make the wireframe, then a method his company uses to print templates from SWx to cut the exact fishmouths. He described it as being quick and accurate. I could not find the article - maybe someone else has the link. Certainly seems to relate directly to this discussion.

[lathropdad]

Mark;

I read the article and still had to get help.

When you do a weldment, SW generates a cut list. Go into that cut list and you will find all the tubes in the weldment. You then can export a single tube to a new drawing. You then have to cut very thin slot though one side of the tube. The last step is to convert the split tube to a sheet metal part and then you can flatten the part using the "flatten" function that is a part of SW sheet metal.

Hope this helps.

[Mark Meredith]

All,
I modeled a complete Scott Tailwheel assembly down to every little part. It was fun but a crazy huge effort! I did it to learn about modeling a complex assembly in Solidworks, and think I achieved my goal even if I fried a few braincells and annoyed my wife. It's based on the original patent drawings, more recent drawings, photos, measurements of the Scott assembly on my Super Chipmunk, and the illustrated parts breakdown from Scott and various vendors. Now on to other things!
It's up on GrabCAD at https://grabcad.com/library/scott-ai...ilwheel-assy-1