What mesh level (in the Wizzard) are you using? (unlikely to get much closer without Mesh set to 8!)
Presume you are looking to simulate flow in the -X direction?!
Good idea to use a plot (cut plot) with velocity vectors turned on to cofirm that you have the flow in the right direction!
mesh level?did you mean result resolution that have number 1~8?.i set it to 6.
and yes.fluid flowing in x direction.
i did set mesh level to 3 and manage to get 1.13 of drag which is better than before.
then i also tried simulate the opposite site of the half bucket which the drag coefficient is larger (2.3).but i didnt get my simulation result near to that.(i got approv. 1.653).
also i tried simulate on plate model(100mmx100mm) but also i didnt got any close result.
here i attach the screenshot of the opposite site halfbucket(drag 2.3) model cut plot.
Looks like you need to refine the grid within the bucket itself and also immediately downstream of it, especially at the outboard (top and bottom) edges. In the real flow, there is a lot of change going on in those sections, so you need to put more gridlines there to properly capture the flow characteristics.
thank you for the reply.
what do you mean by refine the grid within the bucket and dowstream of it?how can i do that?
im sorry im asking too much.but i am really new to this flow simulation.hope you dont mind
Try using a local initial mesh. You'll need to study some training material or tutorials - maybe even the help section has some information - but it does takes some investment of your time and effort, as anyone who uses flow simulation will tell you, to get meaningful results.
But basically to create a local initial mesh, you include a solid object in Solidworks that completely envelopes your part - it's like your part is stuck inside a big cube of Jello. Then you disable that solid object (the big cube of Jello) but then use that same solid object to create a local initial mesh with the correct commands in Flow Simulation As you've mentioned in your response to Karl's suggestion above, refining the mesh will lead to more accurate results. The local initial mesh will help in that regard but will also help avoid having unnecessary cells in areas that you don't need, like far from your part, that would cause excessive run times.
thank for your reply.
so to make a solid object that envelope the part that i need to simulate,i should assemble the part that i want to simulate,inside the solid object?
Yes, there may be better ways to improve your results, but that's what I suggest. Your assembly will consist of two parts, the actual part you're trying to model and then the cube that completely envelopes the actual part. I suggest that you have the 3D envelope extend slightly past the actual part in all three directions, so it's like the actual part is submerged in a block of concrete. Then, make sure you turn off (disable) that block of concrete and apply the local initial mesh conditions to that block of concrete. Those local initial mesh conditions will apply only to that block of concrete and hopefully give you the refinement in mesh where you need it.
You might be able to find more information in Flow Simulation help, maybe even a tutorial...
i did try the thing that you told.but did not getting the drag coefficient right and the mesh is still rough(?).
i set the initial mesh to 3 and getting 1.666+- for drag coefficient instead of 2.3. and getting rough mesh on the part surface.
then i tried to set the initial mesh to 8 and got 1.344+- for drag.but the mesh is better.
plus,when i play the flow trajectories,the flow coming from 2 direction..how to say this.
(imagine a flow on a car,my flow trajectories have flow from front to back of the car and back to front) i dont know if you can understand what i mean.my english is not very good.
so what do you think i do wrong?
Run Simulation as a 2D model, assuming it's infinitely long which is typical for textbook problems. Make sure the surface area reflects actual thickness of CD. Use adaptive mesh refinement, see calculation control options, and make sure the Re number for flow is same as stated in text... be aware of von Karman vortex streaks, the results will not converge. Use tutorial 7 "Flow over a circular cylinder" as a guide.
Note that drag is a very difficult calculation for any CFD package.
In addition to earlier notes above, I think that your computational domain behind the model needs to be extended drastically.
Please see my new post re. "Cylinder Drag"
Adzuan, one point here is that none of understand what 'the text book result' is.
Most of us are assuming that it is test data from a real 'wind tunnel' and then, as Joe said, we further assume that it is just a test on the single bucket section that you have modeled!
If that is the case and like me (returning to 2D from 3D, due to dubious results) your CD (Computational Domain in the FloSim tree) needs to be set at about 15 'object lengths' (OL's) incoming, 25 OL's outgoing and 15 OL's above and below! (12-20 mentioned on ANSYS youtube demos)
These numbers are usually given as chord lengths; 'C' as the aero industry even uses this measurement to define the height (or thickness) of an airfoil/aerofoil/profile/section.
Personally, it seems a little illogical that a 6% (0.06xC) foil and a 24% foil need the same spacing above and below the object, both in a real wind tunel or the same CD setting in CFD.
For foils (2D analysis, 'extrusions'), therefore, I have adopted CD settings, for upper and lower boundaries, which relate to the thickness! (or degree of flow deflection; ie. 15 x t or 15 x 'frontal height')
As you are aware most savonius these days are not 2D 'extrusions' and would therfore experience at least some degree of flow redirection towards the axis! (requiring 3D analysis, equivalent to spanwise flow, like 3D wings with taper and/or twist)
This redirection would most likely require more distant boundaries, above and below, to achieve the same degree of accuracy!
Joe and Karl,
Thank you for your reply.
Yes,i ran the simulation as a 2D model.
I am trying to do what you guys stated above.but just in case.Can i email you guys the model?so that you guys can see what i'm doing wrong,
You can post your model here! Should be an attachment button at the bottom of the 'posters' screen not on my because I'm just a respondent!
Suggest you do it yourself though!
HAVE YOU FOUND THE TUTORIAL(s)? HAVE YOU DONE THE TUTORIAL(s)?
HAVE you read my other post: CYLINDER DRAG today!
LOOK at the mesh! Read my post! As David said several days ago you WILL need to refine the mesh!
There are SEVERAL ways to refine the mesh, Joe was keeping it simple, using automatic settings (which on Initial Mesh 7/8, default to lvl 2 and 2 refinements within the solver and these refinements will no occur till the END of the 2nd and 3rd iteration on the default "automatic" setting!) Search "refine" "mesh refinement"
This WILL refine the mesh inside the 'bucket'!
Read the "cylinder drag", I would imagine you WILL have turbulence (look on youtube at "vortex street" or CFD or 'karman vortex") therefore basicly ignore the non-transient, in the tutorial, go to to the transient!
Also suggest that you search 'drag' on this forum Joe has posted several times before and posted models that you can download!
David said to use "Local Initial Mesh" (LIM's) I said this also and explained in my (brackets, especially for you ) that this is in the FloSim tree!
I included images showing LIM's!
May I ask, where are you?
If you look as Cnu Vasu's posts, you will see some don't get answered!
You are lucky, be careful about using URGENT for some, an assignment could be urgent but it is only urgent for them!
Chinese ofter respond with "I know" when they mean "I understand" or "OK", this can also upset some native speakers, as literally it means "I ALREADY know what you have just tried to teach/explain to me!"
I have an interest in VAWT, solar thermal and Tesla turbines for energy conversion, myself!
I built a Solar Powered car for the first World Solar Challenge!
One problem that some of us have is that we are busy running our own models most of the time (in my case 24 hours and for NO money! In China!)
I can slow down my analysis slightly by using the internet but I do not want to stop a "long run" on a "large model/fine mesh" as it can take the solver many minutes to stop and recover memory etc!
Do you have a CPU/Memory problem (that we are unaware of)?
Attached is another screen shot.
In it you will see;
- D=5m cylinder (BLUE)
- CD (Computational Domain) set far greater than yours (15D front/top/bottom, 25D behind/downstream) along extrusion domain is 0.5m (as per ratio in tutorial!)
- You need similar ratios and I suggest you use 15D/25D NOT 15r/25r (even though r is your object length in the flow stream!)
If you take the EASY path (as suggested two weeks ago by me and recently by Joe);
- go to "Initial mesh" by right mouse clicking "Input Data" in the FloSim tree and selecting "Initial Mesh", set to 7 'auto' (do not NEED narrow channel or THIN WALL sellected) BUT suggest that you can use the THIN WALL and set manually to your bucket wall thickness, this will automatically refine the bucket (NOT downstream/upstream, which will be necessary to get a GOOD result from the auto settings!)
- Mesh 7 and 8 (I believe!) will BOTH default to: set the solver to refine the mesh a minimum of 2 times, ref lvl=2 (splitting EACH initial mesh cell to up, AS the solver deems NECESSARY, to 16 times smaller cells) and will stop the calculation on convergence or at a maximum of 4 travels
IF you DO NOT insert LIM's (shown in the tree in my screen shot) and play with their settings you will almost certainly need to set the solver to ref. lvl=3 and edit the refinement table to include 3 or 4 refinements! (more lines does not mean it will take longer or DO more! The minimum ref=2 sets the MINIMUM the extra lines in the table set the MAXIMUM refinements ONLY (not travels) if the table has 6 refinement points and convergence occurs at 3.7 travels it will NOT use the extra refinement points in the table!
This is as far as I know as simple as it gets!
Let me know how you get on!
To Karl and All the respondent!
I'm sorry if some how i'm making someone here upset or something.
I'm from Malaysia but currently studying in Japan.As you can see my english is not very good.haha.
I AM SORRY!!
I just very new to this Solidworks and Flowsimulation stuff,even now im having hard time to understand the term.I really appriacieate all the responder here.
thank you.Im still trying to do all the suggestion above.
btw,i'm using university computer.i think the computer should be fine?
Again, I AM SORRY!
i'll update again once i tried it Karl!
Appology not necessary!
Better to say "My 'urgent' was not intended to upset!" and the vast majority of us understand that and that English is not your Mother tongue!
I do not think that anyone here would be too upset! Just different values concerning 'urgent'!
The advice concerning 'URGENT' was only intended for the rest of your life!
It is just that I am VERY used to non-native speakers having been born on one continent and lived/worked/traveled to sever others!
I spent two years in Brunei, Labuan and Singapore!
I would say that your computing facilities would be very good in Japan if the University is a genuine one and not some small language College that has obtained permission from a University to use the Universities name!
The latter occurs in Australia frequently, in this World where Education has become something of a 'commercial machine' particularly for foreign students!
Unlike China where youtube is banned: you are free to see "Yuri 1" and cry with me for the inspiration Professor Nito (in Japan) could give to so many here! (Really! Top viewing!) (17 years later the US University students are still trying to catch up with Nito's Yuri 1!)
Nito is more than 20 years my senior and I went through University at a time when the only hard drive was in a special ROOM!
Once, ONE young lady (Chinese) after many years of exchange with others in China, told me that I should not use exclamation marks after my sentences! (She said it was, in her mind, like I was SHOUTING at her or angry with her!)
Hope that I can help to 'inspire you' rather than do it for you!
Hopefully you will learn that "the value in the response USUALLY depends on the way in which the question was asked"!
Or perhaps: "show willing to learn and there are those prepared to assist"!
My point applies to Cnu Vasu's 'bombardment' of posts also!
I get your point Karl
Its not that i want you do it for me,because of my poor english i think it is faster for you and other pro here know the error in my simulation.But i think i can handle it..maybe.Its depressing when the lecturer pushing me to get an accurate result,when i am so new with this FS.
Karl,here the few question i want to ask;
- If i use Reynolds number is approv. 40000 and i didnt check the time dependent in general setting,is that will cause inaccurate of the result that i will get?
- How to take/get the data on the part's surface?.(eg;pressure on the bucket surface)
Thank you in advance!
May I suggest that you scan or take a picture of the text book problem and post it here on this forum. If you post your model, we can suggest and help others who have similar difficulties.
Think my Bosch automotive handbook may be a little better!
Your link quotes as if the Cd is a 'constant'
Cd's ar NOT constants!
Again if you DO or HAD worked through the Cylinder Drag tutorial you would/should have realized that the Cd or drag coefficient (of anything!) is NOT fixed for all speeds! Look at the "getting results" in the .pdf!!
Cylindrical extrusions vary from Cd=60@ Re=0.1 to 0.23@ Re=4e5
Your problem (Cd) will be different BUT will DEFINATELY depend on a)wind speed b)size of the 'bucket' concerned
UNLESS your Professors accept the Cd stated at a particular Reynolds number, you must FIRST define the size of the machine you want to (theoretically) build KNOWING your intended market and the expected wind conditions! (search 'wind map' for this and be prepared to learn about Mr Weibull's work!) http://www.google.ca/url?sa=t&rct=j&q=weibull&source=web&cd=1&ved=0CC8QFjAA&url=http%3A%2F%2Fen.wikipedia.org%2Fwiki%2FWeibull_distribution&ei=04ffTqvyNsOtiQfd1Z21BQ&usg=AFQjCNGpLXviEimiwHNOrKug-KEeDgFr2A&sig2=2AkaJHfI6r35EwrsAkTbQw&cad=rja
On the Time Dependent/Transient I am quite confident that you need this! (As I said look at Votex Street/Karman Vortex on youtube or look for Ropatec's VAWT site, there is a movie there somewhere with a guy doing a CFD simulation and it is DEFINATELY time dependent on the assembly but as the Cylinder Drag 'should' have taught you even object STATIONARY in a STEADY stream CREATE turbulence and Time-Dependent Karman Vortex 'streets' BUT not at ALL Reynolds numbers! (Cylinder not til Re>40)
For whatever its worth Hoerner, Fluid Dynamic Drag, Chapter 3 pg 17, has 2D Cd's at R'numbers between 10^4 & 10^6 as 1.2 for concave down wind and 2.3 for concave up wind (between walls). The numbers stated are for super-critical flows. References are provided
I have absolutely no intention of making a face book account. If you have a scanned copy of Hoerner I would love to get a copy. My copy of the book is getting a bit rickety. If you have the companion book, Fluid Dynamic Lift, I would like that too. I can provide an upload link if you have them. My email is firstname.lastname@example.org. Ping me a note if you could help out with that.
i dont have it either.The link, i googled after you told it in the comment.But I will pm you if i have it
Yes,i had done the cylinder drag once again today,and noticing i did some mistake on the setting.
I'll try again tomorrow for the bucket part.Uni's computer lab open until 9.00pm only.
btw,is your comment here answered the number 2 question?
I have the mesh data..it should be there isnt it?
Sorry lost an your last post!
Your www.unicopter post gave many Cd's (as constants) i.e. did not list the Re numbers for which the Cd's were true!
I covered that in detail up to my wikipedia/weibull link.
Then I covered your question on my (much) earlier statment concerning the need for a Time-Dependent/Transient analysis (rather than a Steady State analysis)
Not sure what you are asking about mesh data!
Time for bed in China 2am!
If the progress in the Solver is still not 100% but the solver is already finished,is that will affecting the result?
I tried again the tutorial with Cylinder (d=0.1m) at Re 1000 and got a good result.(drag = 1.037) but the solver's progress is still at 14%.
here i attached the printscreen of it.
My understanding is that we want need CONVERGED goals (100%=green)
As I use the program I often have goals set that I right clic and chose 'do not use for convergence'
This could be for the reason you are seing: goal axis show little or nothing usuful!
So for example when goals (current value) is 10 or 100 times th Cd I may create an Equation Goal which uses kgf instead of N or even Tonne instead of N! Then I can SEE what is happening as the calculation is progressing! IE the graph has value/function!
The REASON you did not get convergence should be:
- the solver is set to stop after 4 iterations!
- in SW select RUN and 'new calculation'
- a few seconds after completion of the mesh pick PAUSE
- in th SOLVER pick 'calculation' then select 'calculation control options' (this is where you 'tune' the calculation)
- BEFORE I sugested that you set this to:
- (FINISH TAB) min 2 travels (default on Mesh 7/8 but you may not have listened/set to that level!
- (FINISH TAB) max, max, max, max, max ALL off!
- (FINISH TAB) Goals Convergence ON
This means it will do at least 2 refinements (even if coverged BEFORE that!) and then RUN FOR EVER unless the ALL goals that are not set to 'do not use for convergence' actually converge!
- (REFINEMENT TAB) Should be nothing to change IF YOU ARE USING the tutorials boundaries AND the tutorials mesh 7!
- (REFINEMENT TAB) Should have ref lvl=2 and two refinement points in the refinement table(=maximum of 2) if you used mesh 7!!!
Take off the PAUSE!
I disagree; you don't need everything to be green. Convergence is relative. As a user of Flow Simulation, you do have ultimate control on the finish conditions such that everything, if properly set up by user (note: don't always take what the default value the program gives as gospel), then everything should be green. But if it's not all green then it doesn't necessarily mean that it's not finished.
If no goals are set, then for a steady state problem, the internal convergence criteria set by Flow Sim is 4 travels; the default stopping condition for transient is the end time. Going back to SS, 4 travels typically is much more than is needed. One can make the analysis run for a shorter amount of travels, and thus (clock) time, by setting Goals for the analysis. Once those goals, which are important to the user/problem, are below the set tolerance (over the range of the analysis interval), then the goals is acheived 100%. The program will automatically determine a "good" criteria value that it determines, but the user can (and should) check this value and set it manually if it is not proper for the level of sccuracy required (note: select Auto and choose Manual from drop down list that appears, see [ic below)
It's all in the Finish Conditions under the Calculation Control Options (or CCO). You can access the CCO either prior to or during the calcualtion.
I 100% agree with Joe!
Of course you do not need to 'accept' only fully (100%) converged goals!
BUT if you have accepted default (auto) settings that terminate the calculation at the end of 4 travels and the mean line drawn through the oscilations (in a graph with axis zoomed as necessary) particularly on you most important goal(s) AND this mean line has a significant slope to it, you SHOULD be terminating to change the mesh NOT to accept the "result"!
To clarify, a long reasonably level line should be reasonably accurate UNLESS you know refinement is coming and the mesh thus far has been rather 'basic'!