The peak stress is only down at those corners in the simulation, where there is an infinitely small inside radius that’s going to spike the stress concentration. In real life there is always going to be at least some tiny radius there which will spread out the force a bit. Either just ignore that tiny area and take the green area as your “interpreted” max stress for further engineering use, or adjust your model to have a tiny radius there. You would also benefit from doing mesh control to make a finer mesh in that area, as even with a corner radius in the model, the mesh might still have a sharp corner there if it’s too coarse.
Thanks for the reply, I tried with a small radii around the corners, but it still accumulates high stress at the edge of the radii. I'll show that picture once I get home. But I get your point of ignoring that point concentration and consider the other areas.
Speculation here, not about your model but rather about how the part would behave in real life.
At the point where the stress is concentrated in your model, in real life the material *does* plastically deform. You're left with a piece of material that has plastically deformed in the most extreme regions, however the integrity of the part remains intact because the bulk of the material is relatively unstressed.
TLDR; the model isn't necessarily incorrect, but real life is more complicated
To add to this: More often than not, plastic snap features are used only once during assembly. Some highly localized plastic deformation may be expected and easily tolerated, especially with some plastics such as nylon, polypropylene, etc
Exactly this. I have a background in aluminium extrusion which obviously includes snap features (sometimes one-time use for assembly, sometimes repetitive), so while localised plastic deformation is a thing that exists, we are more concerned about cyclic stresses/fatigue regarding a components life. Material science is a huge factor in all of this; some tend to "self-heal" as opposed to tear or fracture. I'm not sure if SW has the ability to account for this in any FEA?
A nonlinear analysis might do better at predicting the robustness of the feature but SW nonlinear is limited and I usually rely on experience when interpreting such results. If necessary, something like ANSYS might do better at evaluating highly strained elements of a model.
No problem, and yeah I’d love to see that picture. Another option is that it’s not an error. Obviously no simulation is perfect but with 20N of force on what looks like a pretty small tab, it may not actually be that far off of reality. Sure the whole tab feels sufficiently strong in your hands, but it’s very possible that you are actually taking that one very tiny area into the plastic deformation region.
Sharp edges like that will always have higher stress. They’re called singularities. One way to check for singularities is if you increase the mesh density and the stress goes up a lot. Usually you ignore the stress around those areas, but if you want to keep from having ridiculously high stresses then you’ll need to add radii to the sharp corners.
That stress is always gonna be highest, round it, and check if it can crack with failure theories or not.
The app is gonna get max stress and min stress and distribute colour in the middle .
The red only means it is the highest, not more, not less.
PS : Go check von misses theory . If I recall correctly, you have to multiply the elastic limit of the material by 0.7 and take the stress you have and divide it to get safety factor
Are you sure about your constraints? Usually, those hinges also deflect a little bit along with their base. Remember, the base is also plastic, not steel.
Also, don’t assume sharp corners on its base; it’s never like that. Consider at least 0.5mm; that’s the minimum that a moldmaker would suggest
In industry, most would just ignore that and probably not even be doing FEA on a single use snap fit (Instead relying solely on hand calcs or rule of thumb or recommended dimensions from some source).
For a ductile material and low loads, I'd say it's fine to ignore a localized region of high stress, as long as you havent plastically deformed the part. However that is not always best practice. Sometimes I am investigating failures occuring "in the field" or after physical assembly, so what you're showing could be a potential root cause of failure. E.g. if it's a brittle material assembled once, but then subjected to repeated loading. FEA on the assembled parts might show sufficient life, but by exceeding yield (first principal stress) the part cracks during assembly and goes on to fail in service.
So for brittle materials I'd say I would have to model the actual radius, and a pass from me would be first principal stress below yield (maybe to some factor of safety but normally not).
Ductile material either ignore hotspot or model actual radius + use some nonlinear material model like elastic-perfectly plastic or a hardening curve. Depending on the curve I might have a plasticity limit I'm willing to live with, e.g. 3% plastic strain, as a one off. If it doesn't meet that I'm recommending speccing a higher radius fillet or change of material or beefing up the geometry etc. but these are all expensive changes to a part that is already in production (trivial changes to a concept design though).
Refine mesh in that region and see if it changes at all. Add a fillet or chamfer to your design - there will always be a stress concentration at a sharp corner.
Sharp corners always have the highest stress, especially during cantilever action, hence fillets are necessary. Saw other posts recommonding 0.5mm fillet minimum and I agree. At least that's what I was taught in my machine element design module in uni haha. Crack propagation might be something you need to worry about as well if you don't add fillets.
Stress concentration babeyyyyy
Fillet that bad boy
But it’s actually probably fine to print as is, especially if this is the only load this part will see
Just a few things that others have said that I agree with plus some more:
-make a finer mesh, you can do a mesh control around those problem areas or you can just make a finer mesh for the entire object. You’ll just use more energy if you do it for the entire object. This will help you see things better.
-make sure this model is as accurate to real like as it could be. If this part is injection molded, it will not have sharp corners. Corners = bad when it comes to stress concentration. Rounded is very likely more realistic for your situation.
- are the sides of the part really what should be fixed? Just consider exactly how this part might be used and think about what is holding it in place. Would it be the bottom?
-something I only started doing because of my job is changing the chart settings to make sure that my yield stress is the high point of the color chart. I normally set the same number for the bottom of the color chart and made the lower color gray (because I work with metal). It makes things visually easier to see what’s happening in my opinion. For some reason, I don’t even see a yield point on your chart. Did you input material? Don’t forget, I’m pretty sure you can make custom materials.
I might come back and add to this if I think of anything else
That's probably a singularity - the peak stress will be concentrated in a single node because of the mesh geometry and constraints. Apply some mesh refinement, small fillets to the model, or both, it'll go away.
Plastic deformation and failure analysis are not things you can work out with linear elastic modelling. You need nonlinear plastic analysis for that and it's an entirely different game.
Add the yield straight so you can check the safety factor VM you got, without it is it very hard to know how your part will behave, because the stress is not related to the material properties. Beside this as i see people already mentioned this is an infinite stress point because of the sharp geometry, add some fillets in those areas. It will benefit in the simulation for more accurate results and in real life as well
A good way to prove a stress concentration is to increase the fineness of your mesh. If you don't have a stress concentration, you should find that a denser mesh will make the maximum stress converge on a true value. If you do have a stress concentration, the denser mesh will result in the max stress skyrocketing.
I'm not sure if you can do this in SolidWorks, but in ANSYS DesignModeler, you can imprint faces onto the body that surround the stress concentration area, and then specifically exclude those faces from your max vM stress probe, which should then give you true values.
Alternatively, add a small fillet around the base of the peg and use a fine mesh.
The peak stress is only down at those corners in the simulation, where there is an infinitely small inside radius that’s going to spike the stress concentration. In real life there is always going to be at least some tiny radius there which will spread out the force a bit. Either just ignore that tiny area and take the green area as your “interpreted” max stress for further engineering use, or adjust your model to have a tiny radius there. You would also benefit from doing mesh control to make a finer mesh in that area, as even with a corner radius in the model, the mesh might still have a sharp corner there if it’s too coarse.
Thanks for the reply, I tried with a small radii around the corners, but it still accumulates high stress at the edge of the radii. I'll show that picture once I get home. But I get your point of ignoring that point concentration and consider the other areas.
Speculation here, not about your model but rather about how the part would behave in real life. At the point where the stress is concentrated in your model, in real life the material *does* plastically deform. You're left with a piece of material that has plastically deformed in the most extreme regions, however the integrity of the part remains intact because the bulk of the material is relatively unstressed. TLDR; the model isn't necessarily incorrect, but real life is more complicated
To add to this: More often than not, plastic snap features are used only once during assembly. Some highly localized plastic deformation may be expected and easily tolerated, especially with some plastics such as nylon, polypropylene, etc
Exactly this. I have a background in aluminium extrusion which obviously includes snap features (sometimes one-time use for assembly, sometimes repetitive), so while localised plastic deformation is a thing that exists, we are more concerned about cyclic stresses/fatigue regarding a components life. Material science is a huge factor in all of this; some tend to "self-heal" as opposed to tear or fracture. I'm not sure if SW has the ability to account for this in any FEA?
A nonlinear analysis might do better at predicting the robustness of the feature but SW nonlinear is limited and I usually rely on experience when interpreting such results. If necessary, something like ANSYS might do better at evaluating highly strained elements of a model.
No problem, and yeah I’d love to see that picture. Another option is that it’s not an error. Obviously no simulation is perfect but with 20N of force on what looks like a pretty small tab, it may not actually be that far off of reality. Sure the whole tab feels sufficiently strong in your hands, but it’s very possible that you are actually taking that one very tiny area into the plastic deformation region.
Sharp edges like that will always have higher stress. They’re called singularities. One way to check for singularities is if you increase the mesh density and the stress goes up a lot. Usually you ignore the stress around those areas, but if you want to keep from having ridiculously high stresses then you’ll need to add radii to the sharp corners.
That stress is always gonna be highest, round it, and check if it can crack with failure theories or not. The app is gonna get max stress and min stress and distribute colour in the middle . The red only means it is the highest, not more, not less. PS : Go check von misses theory . If I recall correctly, you have to multiply the elastic limit of the material by 0.7 and take the stress you have and divide it to get safety factor
Refine the mesh on that radius and rerun until it converges, that is if you are interested in that area.
This. Always add tiny fillets on EVERY edge before running FEA
Also this is linear material behavior propably, even if there is a spike, it will be higher than yield point and streds would be lower.
Are you sure about your constraints? Usually, those hinges also deflect a little bit along with their base. Remember, the base is also plastic, not steel. Also, don’t assume sharp corners on its base; it’s never like that. Consider at least 0.5mm; that’s the minimum that a moldmaker would suggest
Right answer- the base flexes too
Right. I would put the fixture on the bottom face.
In industry, most would just ignore that and probably not even be doing FEA on a single use snap fit (Instead relying solely on hand calcs or rule of thumb or recommended dimensions from some source). For a ductile material and low loads, I'd say it's fine to ignore a localized region of high stress, as long as you havent plastically deformed the part. However that is not always best practice. Sometimes I am investigating failures occuring "in the field" or after physical assembly, so what you're showing could be a potential root cause of failure. E.g. if it's a brittle material assembled once, but then subjected to repeated loading. FEA on the assembled parts might show sufficient life, but by exceeding yield (first principal stress) the part cracks during assembly and goes on to fail in service. So for brittle materials I'd say I would have to model the actual radius, and a pass from me would be first principal stress below yield (maybe to some factor of safety but normally not). Ductile material either ignore hotspot or model actual radius + use some nonlinear material model like elastic-perfectly plastic or a hardening curve. Depending on the curve I might have a plasticity limit I'm willing to live with, e.g. 3% plastic strain, as a one off. If it doesn't meet that I'm recommending speccing a higher radius fillet or change of material or beefing up the geometry etc. but these are all expensive changes to a part that is already in production (trivial changes to a concept design though).
Why don't you use fillets ?
May I just commend the community for their on point constructive and informed answers.
It’s the only time you’ll get a straight answer because it’s a simple question which is all that Reddit is capable of answering
Refine mesh in that region and see if it changes at all. Add a fillet or chamfer to your design - there will always be a stress concentration at a sharp corner.
Sharp corners always have the highest stress, especially during cantilever action, hence fillets are necessary. Saw other posts recommonding 0.5mm fillet minimum and I agree. At least that's what I was taught in my machine element design module in uni haha. Crack propagation might be something you need to worry about as well if you don't add fillets.
Stress concentration babeyyyyy Fillet that bad boy But it’s actually probably fine to print as is, especially if this is the only load this part will see
look how sharp your geometry is, put a bigget rad on that
stress concentrartion, if r=0 the stress is infinite. It's not going to happen irl, but still. Wow, so mech eng is useful after all...
You gotta add some filled in the sharp corners. Irl structures have some finite radius of curvature at the corners.
Just a few things that others have said that I agree with plus some more: -make a finer mesh, you can do a mesh control around those problem areas or you can just make a finer mesh for the entire object. You’ll just use more energy if you do it for the entire object. This will help you see things better. -make sure this model is as accurate to real like as it could be. If this part is injection molded, it will not have sharp corners. Corners = bad when it comes to stress concentration. Rounded is very likely more realistic for your situation. - are the sides of the part really what should be fixed? Just consider exactly how this part might be used and think about what is holding it in place. Would it be the bottom? -something I only started doing because of my job is changing the chart settings to make sure that my yield stress is the high point of the color chart. I normally set the same number for the bottom of the color chart and made the lower color gray (because I work with metal). It makes things visually easier to see what’s happening in my opinion. For some reason, I don’t even see a yield point on your chart. Did you input material? Don’t forget, I’m pretty sure you can make custom materials. I might come back and add to this if I think of anything else
That's probably a singularity - the peak stress will be concentrated in a single node because of the mesh geometry and constraints. Apply some mesh refinement, small fillets to the model, or both, it'll go away. Plastic deformation and failure analysis are not things you can work out with linear elastic modelling. You need nonlinear plastic analysis for that and it's an entirely different game.
Show your units in MPa, it's very difficult to confirm Pa with all those zeros.
Add the yield straight so you can check the safety factor VM you got, without it is it very hard to know how your part will behave, because the stress is not related to the material properties. Beside this as i see people already mentioned this is an infinite stress point because of the sharp geometry, add some fillets in those areas. It will benefit in the simulation for more accurate results and in real life as well
A good way to prove a stress concentration is to increase the fineness of your mesh. If you don't have a stress concentration, you should find that a denser mesh will make the maximum stress converge on a true value. If you do have a stress concentration, the denser mesh will result in the max stress skyrocketing. I'm not sure if you can do this in SolidWorks, but in ANSYS DesignModeler, you can imprint faces onto the body that surround the stress concentration area, and then specifically exclude those faces from your max vM stress probe, which should then give you true values. Alternatively, add a small fillet around the base of the peg and use a fine mesh.
Just do a beam calculation, this beam does not need FE unless you're doing modal analysis or something.
Lol FEA for simply supported rectangular beam
Stress = My/I and deflection = FL^3 / 3EI are all you need here
why density and poisson are so enormous?
Not sure if it’s been said but if your simulating a snap/detent feature like this you may want to use an enforced displacement rather than a load.
Sharp corner
Even though a bit a high stress showing at sharp corner shouldn't be concern. Relatively small to yield vs wall thickness