Accurately modelling Shock Test Fixture

[aetherTap]

Hey everyone,

I'm new to using ANSYS (have experience in COSMOS for Solidworks, though) and I am looking for some guidance.

Our company is needing to meet Shock Test standards and we would like to have a general idea of how a mounted fixture is going to hold up to a specific loading.

In particular, the shear stresses in the bolts are of great concern to us. I suppose my question is pretty general, but I'm wondering the best way to model the bolts and spacers used in order to get the best accuracy while maintaining the dynamic characteristics of such pieces.

For example, in the first picture attached, our bolts are shown with green dots, standard shock test spacers are shown red, and the standard shock test fixture is shown yellow.

Picture 2 shows the test fixture in general, and Picture 3 shows the impact side of the fixture.

 

[Transient1]

It looks like you have a good enough model. I would use the minimum bolt diameter. Contact between adjoing surfaces can be modeled with bonded MPC connections for a first cut. Frictional contact may be neccessary if your worried about shear loads.

 

[aetherTap]

thanks for the reply. yes, I'm thinking frictional contacts between the threaded portions of the bolts, in addition to bolt pre-tensioning, will give me the best results there.


I have another pretty important question regarding this type of analysis: In a Flexible Dynamic analysis, the force of the shock hammer hitting the back of the fixture... would i get the same results using an approximately impulse force like shown in Pic3, or would it be better to model the hammer head and give it a point mass and initial velocity heading towards the fixture?

 

[Transient1]

If you start colliding bodies together, the problem size will get huge quickly. ANSYS can handle it,albiet very slowly. A code like LS-DYNA is better suited to those types of problems.

Additionally, another way of tackling this problem is if your dealing with a sine pulse would be to run a prestressed modal analysis on your fixture. Then you have an idea if it's in the range of your shock excitation. A half sine pulse's dominant frequency is equal to 1/(2*pulse width in seconds). If the fixture is > one octave (twice the frequency of the shock pulse), then it will not experience amplification under the pulse. If you want a hefty factor, ensure the fixture can withstand a static load of 2 times the maximum input acceleration.

Random vibe would be a slightly different method of analyzing.

 

[aetherTap]

OK, I should probably clarify two things:

1) I'm working in the Workbench interface, instead of the full-on ANSYS. I don't have enough experience with that stuff unfortunately.

2) The shock test we're modelling is an impact test where a 400lb hammer swings on a pendulum 5 ft. in radius. Our piece is attached to the standard fixture shown...


I currently have the hammer modelled in Ansys, with a Flexible Dynamic analysis planned. I have calculated the initial velocity of the hammer to be 186.72in/s towards the fixture and I have modelled it 4 in. away (approx. .0214s before impact)

My problem now is that I would like to know how to accurately constrain the impact surfaces (front of hammer and back of main fixture plate)

I have it currently set to augmented lagrangian with a stiffness of 5. damping settings are currently set to the program global default (i believe beta is 0?) the hammer is constrained such that it can only move normal to the main fixture plate (shown in pic3 acting at the center of gravity)

 

[Transient1]

Well the impact surface should be constrained as it is constrained in reality. I have to say I'm not sure about the hammer. There's a couple of things I would try:

First start off with a simpler model, i.e. a thin plate and a square block hammer. Use that as your initial test case.
I think you should be able to allow the hammer to be constrained such that it can only move back and forth. Then after impact it will recoil far into space (assuming that the geoemtry is set up such that it won't fall back on to the plate).

You need to assume some damping greater than 0, check a shock and vibe handbook for estimating damping. That seems like a reasonable stiffness value to start with. You should be using frictionless contact. I was simply giving you another way to solve the problem....ANSYS workbench handles things like pre-stressed modal analysis very easy.

Another way to do this problem would be to smack the plate with the hammer without the test fixture and measure the shock response. You can then input that spectrum in workbench with your test fixture in place and determine its response.

Anyways, good luck.