January 16, 2023 at 6:59 amSuwitcha TitaramSubscriber
Could you please to suggest me ?
I try to use Ansys Explicit dynamic for analysis drop test but i found issued that part no drop to fall.
By I use only standard gravity for analysis data which my part but that part still stay on air.
Then i will try again by create easy model and do it again found easy model can drop.
What difference from both model ?
Could you please to suggest to me ? How i can action this on my part ?
Because i apply same condition from easy model to focus model but it can't drop also.
sample part just like accuator arm can't drop (but only color change)
easy model box animation can drop to fall
January 16, 2023 at 12:39 pmSaiDAnsys Employee
In the first image, the maximum deformation is 2.69e-6 mm whereas in the second image the maximum deformation is 57 mm. You are using "True Scale" in both the cases (see "Result" tab > "Display" options > "1.0 (True Scale)"). It is much easier to see 57 mm than 2.69e-6 mm.
If you want to visualize the deformation in the first case, change "1.0 (True Scale)" to "Auto" or "0.5x Auto".
Hope this helps.
January 16, 2023 at 2:59 pmSuwitcha TitaramSubscriber
Thank you for your answer but really i need to 1st pic part drop to fall and hit with liked base.
But now my part didn't drop to hit with base and that seem stay on air.
Do you know how i can action this ?
January 16, 2023 at 3:40 pmSaiDAnsys Employee
Where is the base in the picture? What is the distance between the part shown in image 1 and the base? Assuming a standard gravity of 9.81 m/s, if the distance between the part and the base is 'x' m, it will take time t1=sqrt(2x/g) seconds to reach the base. So the simulation has to run for at least t1 seconds long. Your End Time (defined in the Analysis Settings) is probably shorter than this. Explicit Dynamics is usually used to simulate events occurring very very short durations, so having a very large t1 is not efficient.
A more efficient way is to recognize that when the part falls freely towards the base, it does not undergo any deformation. The part will deform only when "actual contact or impact" occurs between the part and the base. So a better way to simulate this case is to make the part and the base touch each other and use either "Drop Height" or "Initial Velocity" initial conditions. The initial conditions simulate the fact that when "actual impact" happens between the part and the base, the velocity of the part at the instant of impact is non-zero. This way you don't waste time simulating the free fall of the part since the part undergoes no deformation when it is falling freely.
Hope this helps.
January 16, 2023 at 4:22 pmSuwitcha TitaramSubscriber
An actually i would like to simulation HSA part drop to hit a base for review damage occur on it. and after i apply only std. G ,i didn't seem part animation that part still stay on air also.
and i try to change method as same your recommend by use drop high the animation occur part drop but actual part didn't drop to base also. I change distance between base and part to smaller but animation also same.
Below picture - use drop high method by condition drop 50 mm/s
distance between base vs part around 5 mm
Base set fixed point
(The animation show drop down but part still not hit with my base)
Do you know what issued on this ?
January 16, 2023 at 4:47 pmChris QuanAnsys Employee
It's not clear from the pictures shown if you have applied the Initial Velocity of the drop impact or Drop Height under Initial Conditions.
If not, you need to apply the initial condition to represent the drop.
January 16, 2023 at 5:01 pmSuwitcha TitaramSubscriber
January 16, 2023 at 5:10 pmChris QuanAnsys Employee
January 16, 2023 at 5:28 pmSuwitcha TitaramSubscriber
How i can do for part drop and hit to base ?
Change what parameter ?
January 16, 2023 at 5:38 pmChris QuanAnsys Employee
You need to move the part being dropped very close to the base where it drops onto to reduce the running time of the travel to the base.
The End Time should be long enough to cover its travel time to the base and the event duration of the drop impact.
In your model, I suggest the End Time = 0.005 sec or 0.01 sec or longer, depending upon how far is the distance between the dopped part and the base.
January 16, 2023 at 6:06 pmSuwitcha TitaramSubscriber
Ok i will try to do.
Another question in the same case after i change from initial drop high to use only std. G
i found issued from program show solver energy error.
Could you please suggest ? How i can action this ?
and another question in case i use initial drop high but i selected part only one part at center of body.
After run it complete i found animation show some body do breakout.
What occur on that part ? damage ?
January 16, 2023 at 6:43 pmChris QuanAnsys Employee
Adding Gravity Acceleration keeps adding external work to the system. Thus the total energy is not conserved w.r.t the Reference Energy (initial energy at the Cycle 0). It is expected to see Energy Error if it exceeds 10%.
Setting Energy Reference Cycle under Analysis Settings to a very big number such as 1E7 could prevent the solver interruption by Energy Error.
All objects in the dropped part should have the same initial conditions. Otherwise, the part will break apart before drop impact occurs.
January 18, 2023 at 8:44 amSuwitcha TitaramSubscriber
Could you please adviced from my lasted question ?
January 16, 2023 at 7:10 pmpeteroznewmanSubscriber
The analysis is taking longer than necessary to compute the post-impact deformation and stress because you have left a 5 mm gap between the assembly and the ground surface. SiaD has given you the same advice, but you have not implemented her suggestion correctly.
Move the assembly until it is in contact with the ground and change the drop height to 55 mm. The impact velocity will be calculated for you and the simulation will immediately begin to calculate the deformation due to impact.
Now you might only need an end time of 0.1 s to see the part begin to rebound off the ground. Make sure under Analysis Settings, Output Controls that you have requested 200 frames instead of the default 20 frames of results.
January 17, 2023 at 8:08 amSuwitcha TitaramSubscriber
Thank you for you advice.
I will be try again from your recommend.
An actually i would like to see animation movement more than data calculate because in normally if we free drop part, it will be movement fall down follow gravity.
And i would like to show that animation to my teacher but after i apply same condition in easy model to target model. Target part still stay on air. Then i confuse on this case.
Example easy model that animation show part drop.
But after i apply same condition from easy model to target model but result animation not movement.
How i can do the target model for animation drop as same easy model or not ?
And i have 2 question, Could you please to adviced ?
1. From target model i do transform part from red color to blue color for set condition before analysis.
This case trasform part will be impact from program calculate or not ? (Please adviced)
2. Have difference in program calculate between standard gravity vs initial drop high vs pre-velocity or not ?
And case i use initial drop high, we need to add standard gravity or not ?
The simple model solved to t = 0.147 s so you can see the drop.
The complex model solved to t = 0.0009 s which is such a short time that there is no visible drop. I see that you requested an end time of 0.5 s but I can also see you have set the Output Controls to have Result number of frames to be 50. I told you before to make this a larger number like 500. Why did it only solve for such a short time? Did you stop the solution or was there an error? If it was the Energy Error, you have been told how to fix that above.
- There is no issue using Part Transform to move the part closer to the floor.
- When you use Drop Height, that calculates the initial velocity at t = 0 for you. It assumes the part starts the drop with zero initial velocity. You can have Standard Earth Gravity on in all simulations.
January 18, 2023 at 4:23 pmSuwitcha TitaramSubscriber
If it's not too much trouble, Could you please help me to review my model in attach file ?
How i can do this complex model to drop on base and occur animation or reaction on model ?
Now i try to set model on base and shift it up a bit (2mm) and apply drop high 50 mm/s but after program calculate it still drop a bit and not hit onto base
I don't know why this model occur this result. I try to change every parameter but still show result as same no drop.
(Change time, Change distance,etc)
I would like to my model show animation drop and hit to my base and occur reaction or damage on part that will be make sense for show to my teacher.
The solver stopped because you told it to stop after 1e+6 cycles under Analysis Settings.
The solver spent 161 minutes caluculating 1 million cycles then stopped.
The last few cycles had a time increment of 9e-10 seconds.
Multiply the time increment by 1 million cyles and the calcuation stopped when the simulation time was 9e-4 seconds, but we see it actually got to 7.7e-2 seconds because the time increment was larger at the beginning.
Explicit Dyanamics calcuates the time increment by using the minimum value of a mesh metric called Characteristic Length and other things.
Here is a plot of the Characteristic Length. Notice that the minimum value is 4.6e-6 m but the average value is 4.3e-4, about 100 times larger.
If you remesh the part and increase the Minimum characteristic length by a factor of 100, then you will get a the solution to advance to an end time 100 times longer for the same 1 million cycles.
Replace these two thin solid bodies with a shell mesh on a surface.
These four small bodies are also causing the time increment to be very small.
Removing those six bodies makes the minimum characteristic length be 4.6e-5, a great improvement.
Now the time increment is larger at 7e-9 instead of 9e-10 which is 7.8 times better. It will take about 86 hours to compute to 0.1s, but after 1 million cycles it will be at t=0.007 seconds, then stop unless you change the Maximum number of cycles to 100 million.
Hope this helps.
January 20, 2023 at 7:24 amSuwitcha TitaramSubscriber
Thank you for your adviced.
Now i already try to do model again follow your recommend but i found a bit issued.
Could you please suggest from my below question ?
- I try to do again by re-model increase size around 100x. After run by anasys i found animation already drop but that animation do conflict by part drop unsmoothly. Why my model occur this ? That effected from 4 smaller part ?
How i can action for my part drop to smoothly and direct drop step by step as same 2nd vdo ?
from 2nd VDO i cut other part keep only one and try to analysis again.
The animation show same my requirement.
2. This program calculate from overall part and focus on smaller part than bigger part ?
That will be occur 1st VDO that part will be drop by unsmoothly direct drop because that occur from smaller 4 part ?
Then if i suppress 4 smaller part out will be help to my animation already correct ?