Flat Spring Design Analysis 2

[mirelavus]

Hi all,
I have to design a spring and test it using Pro Mechanica Wildfire 3.
I don't know how should I approach the problem and what will be the boundary conditions. The spring sits between two curved areas. I will attach pictures. Thank you for your postings.

 

[PetieSmo]

mirelavus,

Not precisely sure what your starting condition or input loads are, but from the following article, you can see that the flat spring problem is not a simple one & involves non-linearities, which Mechanica is not generally used to analyze.

http://www.iop.org/EJ/article/1742-6596/.../jpconf9_181_012011.pdf

Maybe with some more information about your application, we could try to be more helpful with simplifications that could help you optimize your design.

PetieSmo

 

[mirelavus]

PetieSmo the article was not found.It was probably removed.
The problem is this: This flat spring has to push in some lugs that sit on a bladder. This bladder when inflated has 80 PSI. The area of the lugs is 2.58in^2.The spring sits between the lugs and a steel tube with 2" ID. Practically the spring sits between two round surfaces. I attached pictures and the initial drawing of the spring. I also attached some hand calculations that make some idealizations: Uniform force and spring bended only on one direction. The space between the two round surfaces is smal: .16", so this will be the preload height of the spring. I calculated the force: F=P*A=80*2.58=206.4 LBF. We will use only 10% of that force: 20.64 LBF. This will be the load that I applied in Mechanica. I is a complicated problem for me, because I only used Mechanica for a very short time. I do not use it in a dayly bases, since we only have one licence at work. Any help will be appreciated. Thank you.

 

[mirelavus]

this is the spring design

 

[mirelavus]

And these are hand calculations

 

[PetieSmo]

Mirelavus,

I've uploaded a copy of the report. Sorry for the bad link.

In searching for some answers to assist you, I stumbled on your Eng-Tips thread from the Spring Engineering forum. In looking at your Mechanica constraints, I have a couple ideas:

1) First of all, I'm wondering if your units are consistent. In one post you stated: "21 LBS or force of 202.96 lbm*in/sec^2)". ProE's default unit system (lbm/in/sec) causes you to have to put in goofy numbers that are off by a factor of 386 inches/sec^2 (1g). I always convert the units system to IPS (inch/lbf/sec) - this way I can clearly input forces in LBF and get stresses out in PSI.
2) Secondly, I can not tell exactly what surface/edge you have selected at the four points that contact the bladder. However, you must be careful about constraining surfaces - if they are over-constrained, you end up preventing that surface from rotating freely, which introduces extra undesirable stiffness.

Let's start with those two things - Let us know how it goes

Pete

 

[mirelavus]

I already have this .pdf file (I've done a lot of research on this subject). The reason I do not follow what is written here is that I don't know if I should make these two contact plates in ProE like an assembly and use this assembly to study the spring in Mechanica, or should I use another approach?
About my units, I first used IPS and then I found some wired units for force, so I switch to metric N-mm-s and I applied -92N instead of 21 LB of force, which is the same thing. The animation does not look how it should, so I know my constraints are wrong. I am trying to apply the force from bellow on the two flat surfaces and fix the bow surface next, to see if I am getting the same result.
About edges selected...that's a problem.

 

[mirelavus]

I attach here my report and as you can see, the max displacemets are about 4 mm (.016"), so the stiffness will be: 92/4=23 N/mm (or 20.64/.016=131 LB/in). My hand calc shows only 43 LB/in with the same thickness. It is true that my hand calc idealize the section, which in reality is not a rectangle. This spring is bended on both directions, but anyway, I don't know if I can trust my FEA results as it is so much difference from hand calc. I will next try to run a sensitivity global and local study and some optimization, maybe I will have a solution that I can trust. ALso, I can see that some elements do not converge even after after 9 passes, so I will probably have to change the mesh size too. Can you tell me if this is trustable? It also fails for the stress because the max allowable is 1100 Mpa for this material. See the attachment as a .zip file. Thank you much.

 

[PetieSmo]

mirelavus,

Can you send a new image of your constraint set? The last image I saw (spring_fea_last.bmp), you had applied 92N to the top AND applied an enforced displacement to each foot (Dx: 1.828mm; Rz:0.8166 rad).

If these are still the constraints, I think you may be double dipping. Either the load will cause the feet to displace OR the enforced displacement of the feet will generate stresses in the spring. Applying both would be a problem.

Here is what I suggest for boundary conditions.
1) Prepare your spring for Quarter symmetry (cut away 3 of the feet, along the Front and Side datums, leaving one-quarter of your spring)
2) Apply 1/4 of your load to the top pad (92/4 = 23N)
3) Apply Symmetry constraints to the faces touching the Front and Side datums - these will take care of your X & Z displacements
4) Constrain the bottom edge of the foot in Y ONLY (note: you might get some localized stresses due to numerical error here, but they can be ignored)
5) Measure your Y displacements (Dy) at the center of the spring and use this to calculate your stiffness (92/Dy N/mm)

If you send the part file, I could give it a go as well.

Good luck!
Peter

 

[mirelavus]

Thank you for your input. That is true, I first applied some other boundery conditions, but then I try to give it another approach. By applying the force from the bottom and fix the bow, you can get the same animation. My conclusion was almost the same both ways: stiffnes=131 LB/in. I run sensitivity local and global today and tomorrow I will run the optimization study. My goal is to maximize the displacements (that means lower stiffnes...I am hoping around 80-90 LB/in) and to minimize the stress (measure <1148 MPa), by changing four variables: height, cutout length and radius of scallopes in a range that gives a regenerable model. After that, I will try your suggestion. Did you look at the report that I sent earlier?

 

[PetieSmo]

mirelavus,

Yes I did look at your report. Looking closer at the video and the details of the report, it appears that you have applied your displacement constraints to the entire upper surface - I think this is where your additional stiffness is coming from. As I mentioned in a previous post, you need to be very judicious when applying displacement constraints to surfaces, as they will generally add rotational stiffness to the model (sometimes it doesn't matter, but for flat springs this is a big deal). Each and every point on this surface is prevented from moving in any direction - this is unrealistic and drives all the deflections and stresses into the legs. This is why I suggested only applying a displacement constraint (NOT a fixed moment) to the bottom edge. Ideally, you would be using a contact interface on the top, which would restrain the surface with normal forces, but no moment; but this is another level of complexity.

You might also read the thread in this forum about Belleville Springs, originally posted by tazengr - the advice given there applies here as well.

One other thing I neglected to mention in my last post:
4b) In the definition of the static analysis, you need to enable the "Large Deflections" checkbox.

Peter

 

[mirelavus]

ok, I give up, would you mind giving it a shot? Here is the part. I am a bigginer in Mechanica so I don't really know what should I expect. I begin my learning with a difficult part...but it is what it is.
Thank you much and I am looking forward for your foundings.

 

[mirelavus]

Here is the second report, where I tried some of your sugestions. think i am getting closer. What do you think?
I need stiffnes around 80-90lb/in at a preload height of .16".

 

[PetieSmo]

mirelavus,

Your deflected shape looks much more believable. Based on your results, it appears you got:
92N / 6.27mm = 14.67 N/mm ~ 83.7 lbf/in

However, your vonMises stresses are ~275ksi

So, yes, I think you're getting closer to having a believable model. Once you get that, I think you can start doing the optimization for a final design.

Peter

PS I will try and run my symmetry version sometime today - just for comparison.

 

[mirelavus]

I run the optimization and after 11th iterations I stopped it, because it took too much time (already 2 hours). I got the stress down to 1147 MPa (1148 MPa is the yield point). I set the goal: maximize displacemets by keeping the stress < 1140 MPa (which is the yield point), by modifying almost all parameters with exception to cutout width (which I don't want to change). The thing is after all these iterations I got the new stiffness around 130 LB/in for displacements around 4 mm. I don't think I got to run 20 iterations to see where this is going. I either have to find a material that has the yield above 1200 MPa and the thickness around .56 mm (.022"), or to leave with having the stress extremely close to yield (1147 MPa < 1148MPa).
Keep me posted about your foundings when you have time.
It's hard to believe that my flat spring has now 130 LB/in, but it is what Pro Mechanica tells me. Should I trust it?
What's your opinion on this?
Thank you much

 

[PetieSmo]

Mirelavus,

I did a couple runs in WF4 - sorry for the poor image quality in the report.

As you can see, the displacement constraints make a big difference!
Constraining the whole edge prevents rotation of the foot about the X axis giving spring constant ~65 lbf/in

Constraining only the corner against Y displacements allows that bottom edge to rotate and softens the result to about 33 lbf/in.

These two answers bound the approximate results computed by hand by desertfox. Also, the geometry has changed slightly since desertfox did his calcs. I think I've got the model in the ball park, but as you can see, the stresses are still way too high.

Good luck
Peter

 

[mirelavus]

I don't want any rotation to happen, so the first analysis looks closer to mine (which was around 80 LB/in, but I fixed it on y direction instead of giving it a zero value. Whahave you done for rotational constraints in the first case (analysis 1)? I fixed it on Dy and Ry. Maybe I would have to change this into zeros? I never knew what is the difference between zero and fixed. I know it makes a huge difference what edges, points or surfaces do you pick and also what conditions (constraints) do you apply. That's why I posted the thread, because every time I picked another surface or edge, Pro Mechanica would give me a different answer, so I did not know what I suppose to pick anymore. My experience with FEA is at the beginer level so I do not know what should I expect either. Now I know a little more about it and I got a little more confidence and idea of what to expect and what is closer to reality.
desertfox idealized the cross section of the spring (like I did in my hand calculations) and get almost the same solutions as I got, but in Pro Mechanica, the real part gave me different answers, so I knew that something was wrong with my boundary conditions, that's why I did this post. Thank you much.

 

[PetieSmo]

mirelavus,

Q: "What have you done for rotational constraints in the first case (analysis 1)?:
A: I released the rotational constraints. My only constraint was Dy:Fixed (It is the same constraint type as shown for Analysis 2, I just selected an edge rather than a single point).

Q: "I never knew what is the difference between zero and fixed."
A: There is no difference between Dy=0 and Dy=Fixed.

Q: "My experience with FEA is at the beginer level so I do not know what should I expect either."
A: I would recommend running some simple analyses that you can easily check against hand calculations (e.g., flat plates, beams, bolted assembly, etc...). Try different boundary conditions and see how your errors change from theoretical. This will start to give you a sense of how to set up your problems. Analysis with FEA is much more than just running a software package - it's a skill that demands an understanding of the physics and when the software is giving you a bogus answer.

Best of luck in your endeavors,

Peter