copper coil around a shaft 1

[nekojita]

Hi,

I want to model the transient heat transfer characteristics of:

a zero pitch coil (30 gauge polyimide copper wire, 10 mm long) wound on a hollow cylinder (nylon tube 2.5mm OD, 0.5mm ID). The coil has a very thin layer of polyolefin over it. (.05mm). Two additional layers will contact the polyolefin acting as the q out for the coil, the first, 0.5mm thick, the second, 2.0mm.

In this model, the coil will be set for constant temperature.

I have the the following questions:

1) How to create the model of the round wire on the shaft material? (3D)

2) How to create scenarios where the thin layer of polyolefin is conformal to the coil and also where there are air gaps because the polyolefin does not conform to the shape of the coil.

3) How to create the layer in contact with the polyolefin that is uniform,i.e., entire area has same q out? The q out is not constant with areas of higher and lower q out?

Thanks,

Art

 

[nekojita]

I thought that I had a solution to creating the coil described in my earlier post by starting with a solid torus. I then copied the tori in groups and ultimately added them together over the a partial length of the shaft. (hollow cylinder)

What I got was a horrifically slow workspace and a gigantic .db file.

There must be a better way to make a coil. Springs are quite common in mechanical models, however, I don't see a solid helix available through the Ansys GUI.

Does any have a suggestion?

Thanks,

Art

 

[cloche]

Art,
you'd better simplify your problem by setting up an axisymmetric model of your pipe+coil. This would be a 2D model and so would be extremely lightweigth and fast. Mesh the 2D axisymmetric section with planar elements by activating the "axisymmetric" option.
The Verification Manual gives several examples that could fit your needs: VM105, VM172, VM102, and moreover VM168.

Claudio

 

[Drej]

Claudio - Am I misreading what you said, or are you suggesting an axisymmetric model of a helical coil? All of the verication examples you've suggested are axisymmetric candidates because of appropriate geometry, but the helical coil however is absolutely not axisymmetric. On the other hand, are you suggesting that the coil be simplified to a cylinder, and then an axisymmetric model completed of this? This would be more appropriate.

Art - Regarding the issue of creating a torus/helix within the ANSYS GUI there is no dedicated geometry tool available for this. However, it is possible using some clever APDL to write the geometry out in terms of helical equations. Check out the macros below (try each and modify to your needs) which create a helix using this method.

Cheers,

-- drej --

! ************************
! HELICAL SPRING MACRO (1)
! helix
! radius = arg1
! pitch = arg2
! number of coils= arg3

r=arg1
p=arg2
n=arg3
tlen=arg3*arg2

/prep7

*get,mxkp,kp,,num,max

csys,0
*afun,rad
pi=acos(-1)
*do,i,1,(4*n+1),1
kpno=mxkp+i
x=r*cos((i-1)*(pi/2))
y=r*sin((i-1)*(pi/2))
z=tlen*((i-1)/(4*n))
k,kpno,x,y,z
*enddo
csys,1
krotate,all
l,mxkp+1,mxkp+2
*repeat,(4*n),1,1
csys,0
! END
! ************************



! ************************
! HELICAL SPRING MACRO (2)
/PREP7

MULTIPRO,'START',5
*CSET,1,3,ODS,'OUTER DIAMETER OF SPRING',20
*CSET,4,6,DSW,'DIAMETER OF SPRING WIRE',2
*CSET,7,9,NAC,'NUMBER OF ACTIVE COILS',8
*CSET,10,12,FLS,'FREE LENGTH OF SPRING',20
*CSET,13,15,KPR,'KEYPOINT ANGULAR DISTANCE',5
*CSET,61,62,'SPRING DATA INPUT'
*CSET,63,64,'MACRO BY HURSHA S. NARAYAN'
MULTIPRO,'END'

!Mean Diameter of Spring
MDS = ODS-DSW

!Degrees to Radians
D2R = ACOS(-1.0)/180

!Coil Pitch
COILP = FLS/NAC

!TOTAL NUMBER OF KEYPOINTS
KEYT = 360*NAC/KPR + 1

*IF,KEYT,GT,200,THEN
KEYT= 200
KPR = 360*NAC/(KEYT-1)
*ENDIF

*DO,I,1,KEYT,1
THETA=(I-1)*KPR*D2R
K,I,0.5*MDS*COS(THETA),0.5*MDS*SIN(THETA),THETA*COILP/(2.0*ACOS(-1.0))
*ENDDO

BSPLINE,ALL

K,KEYT+1,KX(1)+10,KY(1),KZ(1)
K,KEYT+2,KX(1),KY(1),KZ(1)+10

WPLANE,1,KX(1),KY(1),KZ(1),KX(KEYT+1),KY(KEYT+1),KZ(KEYT+1),KX(KEYT+2),K
Y(KEYT+2),KZ(KEYT+2)

CYL4,0,0,0.5*DSW

VDRAG,1,,,,,,1

WPCSYS,1,0

WPSTYLE,,,,,,,,0

/VIEW,1,0,0,1

VPLOT

ET,1,185

ESIZE,DSW/5.0

VSWEEP,1,1,6,1
! ************************


Also try this:

http://ansys.net/ansys/input/spring.inp

------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cloche]

Of course the helix is not axisymmetric, but as regards electromagnetic properties of the circuit it has absolutely no importance and can be modeled as a cylinder. Also in the VM examples a lot of solenoids are approximated as cylindrical uniform windings.
I suppose from what Art is saying that he is not interested in local electromagnetic field analysis (in which case approximating the coil with a cylinder would be inappropriate as current intensity vectors would not be correctly oriented). I'm assuming he is interested in the overall properties of the coil winding, and from a thermal point of view also I believe that the cylindrical approx can fit his needs: only model 1 "turn" of the "cylindricated" winding in 2D axisymmetric, with all the details needed (layer of polyolephin, copper wire, section of the cylindrical support pipe). If boundary effects at the coil's extremities must be included, the axisymm model can be extended to the full length of the coil + extra-length of the support pipe.

I agree that a complete 3D model of the coil made with swept meshes (one for the copper wire and one for the anulus of insulation polyolephin...) along an helix is super-perfect, but are you sure you won't need a CRAY MP-4 to run the scenarios without getting a white beard? ;-)

Claudio

 

[nekojita]

Claudio, Drej:

Thanks for yours posts and comments. Drej, I did try the spring macros: the first produced a very simplistic helix; was not sure how to start the second which uses multipro.

The spring.inp file loaded, ran, then crashed during the solution. Don't know what to make of that.

Since I am a total newbie with APDL, it's hard to figure out how to even begin editing macros.

I am thinking that I may drop back to a 2D model to see what I can learn.

Any comments?

Thanks,

Art

 

[Drej]

Art,

All three macros work fine on my machine (the second macro takes about 1.5 minutes to mesh), but I guess if you're not familiar with APDL like you say, it will be difficult for you. If you would like to get the second macro to work, you must copy/paste it all to a text file and save it. Then from ANSYS go to File > Read input as... > and read in the file. This is the same for any macro - it should always be saved in a file and read in (you can paste it in to the command line, but there are certain difficultites with doing that), ALSO; I have noticed on the second macro that the line:

WPLANE,1,KX(1),KY(1),KZ(1),KX(KEYT+1),KY(KEYT+1),KZ(KEYT+1),KX(KEYT+2),K
Y(KEYT+2),KZ(KEYT+2)

should be all one line such as:

WPLANE,1,KX(1),KY(1),KZ(1),KX(KEYT+1),KY(KEYT+1),KZ(KEYT+1),KX(KEYT+2),KY(KEYT+2),KZ(KEYT+2)

As Claudio pointed out earlier, you may be well advised to drop back to 2D with something very simple - starting simple in a complex physical model is always the best thing to do. Let me know if you need any more help with macros.

Cheers,

-- drej --


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[nekojita]

Drej,

I was able to get the 2nd macro to load after correcting the syntax on the wrapped line. So far, I have diasbled the meshing but have another curious problem. The dimensions of that example coil are downright huge. If I scale the dimensions to my world, I get lots of errors. I have scaled it as shown below:

20 ----> .002
2 ----> .0002
8 ----> 50
20 ----> .002
5 ----> .05

When I select the parameters shown above, I get the message: "resulting offset curve would have cusps. Offset not possible."

Also, when I change the spring length I get the same error. Seems that this macro is either not robust or I am missing something.

Hopefully you have some enlightening comments.

Thanks,

Art

 

[cloche]

Didn't have time to carefully read the macros, but the principle seems clear. There is one dimension that should be "scale-independent": the angular spacing "KPR". Scaling it down to 0.05° from 5° could become incompatible with other definition parameters (do you really need one spline defpoint for each 0.05° of revolution?). Ansys has limitations on the number of defpoints per spline, so the macro controls it by forcing a max number of defpoints to 200; in this case, anyway, with 50 turns you have a KPR of 89.55°, which is huge and very likely leads the spline to have cuspids (i.e., brutal tangency / curvature discontinuities).
Suggestion: split the "single-spline" coil into n pieces; for each n-th segment, run the macro. Make the successive runs of the macro start from where the previous ends (a bit of math calculation is necessary...). Then add the volumes altogether if you want a single solid (don't see if it would really be necessary).

Claudio

 

[Drej]

Art,

Yeah the dimensions could be huge, depends on the units you use, but the default parameters are in millimetres. I think I've found your problem, though. We just need to be practical in terms of the numbers we feed into the program. Here are the thress sets of numbers:

(default --> yours --> mine)

20 ----> .002 ----> .002
2 ----> .0002 ----> .0002
8 ----> 50 ----> 50
20 ----> .002 ----> .2
5 ----> .05 ----> .05

And these are:

OUTER DIAMETER OF SPRING
DIAMETER OF SPRING WIRE
NUMBER OF ACTIVE COILS
FREE LENGTH OF SPRING
KEYPOINT ANGULAR DISTANCE

I've just made the free length of the spring a practical value, whereas previously you had made this equal to the outer diameter with 50 turns of the coil! The geometry couldn't fit into that small space, which is why you had the "resulting offset curve would have cusps" error. My advice is to just play with it a bit more, it's an excellent macro and is very robust from my experience.

Cheers,

-- drej --


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[nekojita]

Drej,

Thanks...I see that it doesn't fit now. How did you know that the default parameters are in millimetres? I assumed default SI units that's why I thought the default values made such large coils.

Also, is there a way to check dimensions on an object that has been created in the workplane? (show a grid?) Or to display reference dimensions either in the workplane or on an output plot? Seems that I don't have a handy way to do a sanity check on object dimensions.

Art

 

[Drej]

There are a number of ways to check dimensions on an object. These are:

Command - description
---------------------------

alist,p - pick the area, the box will show you its properties
llist,p - pick the line, it will show you the length in the dialogue box
kdist,p - pick the two keypoints, it will tell you the distances
ndist,p - same as kdist but with nodes

You can display a grid based on the working plane - check the help file for that.

The default units for that spring was in mm (I know the guy who did it), but they could equally be in inches, miles, km, metres... anything you want as long as they're all consistent it doesn't matter.

Cheers,

-- drej --


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[nekojita]

Drej,

Thanks. What line in the macro describes setting the default parameters in millimetres? I don't see that.

Art

 

[cloche]

Art,
there is no specification of the unit in a macro, since in ANSYS the units are arbitrary. As Drej said, you only have to keep consistent with your system: for example, if you want to work in mm, mass unit will be ton, density in ton/mm^3 (that is, water has a density of 1.000E-9), pressure in N/mm^2=MPa, force in N, acceleration in mm/s^2, etc... There is a chapter of the Help describing the principal consistent systems of units multipliers. If your case is not in those described, simply do some dimensional analysis to find out the whole series of derived units.
As another example, imagine you have a square of 1m size; you can set up the corners in ANSYS as {1;0},{1;1},{0;1},{0;0} if you "think in meters", or as {3;0} etc if you "think in feet", or as {1000;0} etc if you "think in millimeters", etc etc! Of course, when you begin a model in your own way and then you run a macro created in another context, dimensions can be an issue, since you won't be able to know to which unit this other context refered.

Drej,
sorry for my unuseful previous post; if I had paid more attention to the macro I wouldn't have written "for nothing"...

Bye to all!

Claudio

 

[Drej]

It doesn't specifically say that in the macro. Remember that in FEA you make your set of units, based on a consistent system.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cloche]

<<... in FEA you make your set of units, based on...>>

Ehm, it's better 2 say "in ANSYS you make your set of units".
This is not a general statement: Cosmos/M for example uses explicit sets of units. Also Algor does. Generally all FEMs that directly "connect" to a CAD uses the CAD file's length units when specified. Of course, the choice of a unit system always rely on the designer, not on the program...

Claudio

 

[Drej]

1.) In FEA you create an analysis based on your own unit system. Always. Every time. This is indeed a general statement.

2.) However, in some FE packages, they provide a set of units for you to work to when you import CAD geometry or when you start your geometry from scratch (such as ANSYS DesignModeller). This is different.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cloche]

Drej,
sorry to become a bit polemical, but even if I like very much yor technical preparation and your wise indications (really), permit me to say that I dislike the tone you generally use.
So, for the units: do you want me to write a paper about Buckingham theorem? Do you really think it's useful??!??? Do you think it will help people like Art that still don't have these concepts perfectly clear probably because they come from another software, like, just to repeat with examples I KNOW (I USED THEM), Cosmos and Algor? <Art, no offence: I myself got confused with Ansys the first times I used it at the university>. USE THESE SOFTWARES AND I REALLY WONDER IF YOU WILL BE DISCUSSING AGAIN ON HOW MUCH "THIS IS DIFFERENT", and now you HAVE to explain us EXACTLY WHY "this is different". Ansys family of products may be different. In Ansys Multiphysics I do can mix up my ARBITRARY units, so that if I don't pay attention I'll get a totally unconsistent system; in Cosmos I CAN NOT: each time I enter a value I have to dimension it. I'm allowed to give a density in grams/cubic micron even if my lengths are in kilometers, but the program WILL INTERNALLY CONVERT ALL THIS. It's this lack of guidelines in Ansys that get the users disoriented at first.
It's exactly like with the helix simplified with an axisymm: consider me idiot if you please (I DO KNOW THAT AN HELIX IS AN HELIX, DO YOU WANT ME TO POST A PAPER ABOUT 3D PARAMETRIC CURVES? Already done: see the forums about Unigraphics), but we are supposed to be engineers, not mathematicians. So in our replies, from now on and in whatever forum, please could we keep this in mind (me first, I recognize).

 

[nekojita]

All,

With all being said about units and consistent units, how do I know at a glance what units my current worksheet (I might be continuing work on it a week later) or someone else's worksheet when I open it up?

Drej, how did you know that the defaults for the coils were in millimeters?

Art

 

[cloche]

Art,
I'm afraid you have no way to know "in which" unit system you are. That makes no importance, provided that everything (lengths, masses, forces, pressures, densities, times,...) is consistent. By consistent I mean that it respects the dimensional analysis principles ([F]=[m][l]/[t]^2 etc...). Another example: imagine you open a database created by someone else, and read the coordinates of a keypoint: {0.478;-0.059}; are these values in meters or what? Well, that has no importance; if you interprete them as meters, and you suppose that time is in seconds and force in Newton, you will expect density to be expressed somewhat like xxxxE+0, whether if you interprete them as millimeters the density is x.xxE-9. The physical "real world" size would not be the same, but from an analysis point of view it's the same.
Of course, when it deals with objects and studies you have knowledge upon, you already can guess which are the "most probable" units: in turbomachinery, which is my field, when I read "x.xxx" for the coordinates all over a model then I reasonably know that the length unit is meter (a turbine could not be x.xxx mm big, nor x.xxx kilometers), or when I see yyyy all over another model I then know that it's in millimeters. Of course, if somebody wants to play a trick on me and gives a file in centimeters, then it will be a little bit more difficult at the first glance! ;-).
I hope I didn't confuse you even more... and that all this is sufficiently "appropriate". If not, I'm sure "someone else" will correct.

Claudio