Dear all,
I am doing 2-D simulation of pilgering process in Abaqus. I have modelled 3 parts:- Die, mandrel and tube as shown in figure attached.Image "pilger 3D" is 3D model of pilgering process. I am making this in 2-D i.e., I am modelling only central plane for simulation while it is axisymmetric at mandrel central axis see image "pilgering 2D" attached.
Die moves to and fro in this process and after each stroke tube is fed and turned.
Die reciprocates at 60 strokes/minute. Stroke length=440 mm. Feed = 3.4 mm/stroke.
Die and mandrel are rigid while tube is deformable.
Tube material is Zircaloy-4.
I have to do 150 strokes of die but after around 50 strokes my job is getting aborted. I think due to excessive mesh distortion.
I am using static,general step to give all boundary conditions.
Please see attached image file "result pilgering 2D".
Please suggest what should be done should I refine my mesh, change element type or use explicit method.
Kindly help me.
Regards,
Ayan Jain
What you have there is a beautiful example of a classical error, called "hourglassing".
You have used linear reduced integration elements which are very sensitive to this behaviour. Have a look at ch. 4.1 in the getting started manual to understand what this means.
You can shift to fully integrated elements or perhaps even better to quadratic elements.
Please also note that your mesh es extremely coarse in the vertical direction, you will not be able to capture the full behaviour of a rolling process this way (where the stress gradient in vertical direction may be large).
What you have there is a beautiful example of a classical error, called "hourglassing".
You have used linear reduced integration elements which are very sensitive to this behaviour. Have a look at ch. 4.1 in the getting started manual to understand what this means.
You can shift to fully integrated elements or perhaps even better to quadratic elements.
Please also note that your mesh es extremely coarse in the vertical direction, you will not be able to capture the full behaviour of a rolling process this way (where the stress gradient in vertical direction may be large).
Dear Ayan,
I would second the opinion of Mr. Baeker and would like to add some points.
1. This is first of all an "Hourglass" problem as mentioned. Each FEM software provides some measures to overcome this effect. It can happen with both Shell or solid elements and could be avoided by making the elements stiffer. With stiffer elements, the boundaries of elements themselves do not distort under the loading. With this it means, you might want to use different element type or use different integration scheme for the same element.
2. For the element size, a general rule of thumb is minimum 5 elements over the thickness and minimum 8 element for a 90 degrees of bend. I would suggest to use adaptive remeshing to reduce the element size (if possible only) at the location where your tools come in contact with the part. Refining the mesh would lead to a better distribution (in general) of the post processing quantities. For that you might also need to do a mesh convergence analysis so that your results are independent of mesh size.
3. Please also check the value of friction coefficient that is being used in the contact settings. You can study its influence by setting it as a very small value. Alternatively you might want to use different contact type.
Please update if you still get problems after the modifications.
regards,
Hamad
- Badges
- Science topic