Ansys analysis of the frame

[vasily]

hello
We are trying to analyze our frame using ansys. For our elements we are using BEAM4 and PIPE16. The file solves with out any problems, however we can't find a way to see what is the stress distribution in our members and where is the highest stress is concentrated at. I'm refereing to von Mises stresses and Principle stresses.

thanks
vas
Temple University

[vasily]

hello
We are trying to analyze our frame using ansys. For our elements we are using BEAM4 and PIPE16. The file solves with out any problems, however we can't find a way to see what is the stress distribution in our members and where is the highest stress is concentrated at. I'm refereing to von Mises stresses and Principle stresses.

thanks
vas
Temple University

[Steve Yao]

I would recommend you model the entire frame with the Beam4 elements, or all PIPE16 elements to maintain consistent behavior throughout the model.

Also you cannot see the stress distribution using the contour plot results because the Beam4 elements are lines, and have no contours. Look up "Beam4" in the Help. Table 4.3 lists the output quantities available with the Beam4 element.

You are probably interested in SMAX, Maximum Stress (direct stress + bending stress). Note: there are no Von Mises or principal stresses for a line element like Beam4.

In order to plot SMAX you must do the following(Assuming Ansys 10 classic (non-Workbench):
[]General Postproc>>Element Table>>Define Table
[]Add
Set label: "SMAX_i"
Set Data Item: "By sequence num"
In the list to the right, Select: "NMISC,"
In the field below that, enter: "NMISC, 1"
[]Click "ok"

[ADD] another table item with label "SMAX_j" and item "NMISC, 3"

When you are done defining the table, hit [CLOSE]

Hit General Postproc>>Element Table>>Plot ELem Table

Select which element table item you want to plot form the first pull-down menu and [OK]

Hope that helps.

[Garry C]

As a follow up question,
I'm also analysing our spaceframe in ANSYS. I've used BEAM189 elements throughout. I can plot the stress contours on the element shapes (using the /eshape command). This can give me a plot of the von-mises stress on each beam element.
However want I really want is to list the max v-m stress for each line element, not for each node. I've meshed it so that each line is divided into 20 elements, and at each of these points the BEAM189 element for the sections i'm using have 8 nodes, so thats a ridculous number of nodes and the results, although nice and colourful, aren't very easy to interpret. By getting the max stress in each Line this will correspond to the max stresses in each tube of the spaceframe.

Thanks in advance

[Jersey Tom]

Chassis follows design for stiffness, not design for ultimate strength. With the safety rules the chassis are all way overbuilt from a stress standpoint.

[vasily]

Thank you for the advice, I'll try this in the next couple of hours and will let you know of the results.
Jersey Tom, I do understand that if the guidelines are followed the frame will be strong enough anyway. But from design event point of view it won't hurt to show the judges stress analysis. In my opinion it's always better to over analyze rather then not analyze enough (as long as it doesn't take up that much more time).

V

[Steve Yao]

Tom is not saying that analysis is unnecessary. In fact, I am sure he actually a big advocate.

What he is trying to get at is that chassis performance on track is not dictated by how strong it is(unless you are crashing into something), but rather how stiff it is.

So run the FEA (careful not to over-constrain the model), and of course ensure it is strong enough, but also pay close attention to deflections.

[vasily]

An update
I used the maximum stress command to analyze the frame using Beam4, and it worked. I got about max of 5400 psi. What do you think of this number?
I also tried to run the frame with beam 189, but it seems you can only analyze one kind of tube at once (for example .065 tube). Unless I missed something when I was reading the help files.
And don't get me wrong, I'm definitely checking the frame for torsional stiffness. So far we have a max deflection of about .6in, with torsional stiffness of about 2500lb*ft/deg. So we are trying other options to make that a better number.
Thanks for the help
V
Temple University

[Jersey Tom]

What do I think of 5.4ksi stress? I dunno. What do you think of it? What is the yield stress of your chassis material in the as-supplied state? Welded? Actual bead strength?

2500 ft*lbf / deg.. do you feel this is sufficient, or its low, or its high? Based on what?

How much is it expected to weigh for 2500 ft*lbf / deg?

[clark]

i also think this is low value. we are currently having abt 5000lb-feet/deg. but then u need to have a proper co ordination with ur suspension. if suspension is stiff enough ,then it can be okay

[pentek123456]

we used beam 188. What is the diff between beam 118 and 189. and how are other teams analyzing their chassis. As in what forces are you appling where. Many teams have different ways of doing torsion test. I think torsion test is way overrated and becasue of that many teams end up overbuilding the chassis.