I am trying to do deep drawing in ABAQUS. While to do this, I'm getting help to ABAQUS examples which is name Deep Drawing a Square Box. In my model look everything is ok. But my punch reaction force is very low. In addition I did this model experiment in our laboratory. For example my model max punch force 4000 N but in experiment real punch force for same material nearly 12000 N.Are there any mistake on my model? My model link is below:
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Abaqus 3d Deep Drawing 1
- Thread starter IMOTEC
- Start date
-
1
- #2
- Thread starter
- #3
Thank you for your interest. I Will try what you say. But there is one more thing. Thé Force not only the problem. For example When i change friction coefficient there is nothing to change or When i changed young module also nothing change. I didn't understand where is problem. I must solve This please help më.
IceBreakerSours
Bioengineer
I have not looked at your model but to prevent one of the common mistakes make sure, just in case, that your units are consistent.
Are you new to this forum? If so, please read these FAQ:
Are you new to this forum? If so, please read these FAQ:
- Thread starter
- #5
I am süre that my units are consistent. I used Pascal , meter , and Newton. I check All units. There should be different problem but where is the problem. Even if my force is mistake, When i change something there must be change something .Please check my model and try to change something then you understand what i am talking about.
I changed the model to an axisymmetric case but replaced the load on the holder by a fixed restraint, and removed friction, and also changed the step to a static general case. I'm not sure why you chose dynamic explicit other than it may have been easier to run. Eventually the model ran using a small initial time step and reducing the minimum time step to 1e-9, and I got just over 12000N as the reaction force on the punch. All of your units are consistent with steel and presumably the yield stress is correct. How you got 4000N in your model I don't know, unless it didn't actually finish the step before the job aborted. Anyway, your experimental results are correct.
- Thread starter
- #9
Axisymmetric model is not correct for my problem because my deep drawn part is square and I changed the other simulation my model. For example first part 60x60 mm2 which i send you. And other model my part reduce 60x50 mm2 and other 60x40 and this goes like this. Punch and die is ok. It can be axisymmetric. But the other thing must be 3D. The other thing why i choose explicit: because i tried before standard but i got error "too many increment needed" and also it need too many BC and step. So i didn't understand main idea of standard. But explicit is easier than standard in my opinion. Every thing looks ok in my model but it didn't effect change of friction or elastic modulus. MY reaction force and experiment force, and model picture links are below.
Even though the blank is square you can see from your stress distribution that the results are axisymmetric by nature. Most of the work carried out on the blank occurs within the die area and the back end of the blank (the square end) doesn't seem to do much, and also doesn't move much as the punch is moved down. That may be why changing friction doesn't have much of an effect as the blank seems to be effectively restrained within the holder.
Explicit does work better when you have contact and elastic plastic material as the stability conditions aren't rigorously enforced. In the static analysis I ran there were problems reaching the final time with not enough increments and so on, but if you include contact controls and the right time step then it runs and runs much quicker than an explicit analysis.
In your model you have shell elements. How these behave when you have stresses exceeding yield through part of the thickness I'm not sure of. In the 2D axisymmetric model I ran, I could model the actual thickness and non linear stress distribution through that. Perhaps changing the elements in the 3D model to brick elements might produce better results, though this would be expensive computationally if you include enough elements through the thickness.
If your experimental results differ significantly for the different size blanks then use a 3D model but as a first step, and as a means of understanding the general behaviour, I'd recommend using a 2D axisymmetric model first. This can be generated relatively quickly from your existing 3D geometry. Using a 2D approach means you can assess the sensitivity of the results to changing various factors, such as element types, friction,etc. and also get results in a matter of minutes. Then try running the full kit and caboodle 3D model.
Explicit does work better when you have contact and elastic plastic material as the stability conditions aren't rigorously enforced. In the static analysis I ran there were problems reaching the final time with not enough increments and so on, but if you include contact controls and the right time step then it runs and runs much quicker than an explicit analysis.
In your model you have shell elements. How these behave when you have stresses exceeding yield through part of the thickness I'm not sure of. In the 2D axisymmetric model I ran, I could model the actual thickness and non linear stress distribution through that. Perhaps changing the elements in the 3D model to brick elements might produce better results, though this would be expensive computationally if you include enough elements through the thickness.
If your experimental results differ significantly for the different size blanks then use a 3D model but as a first step, and as a means of understanding the general behaviour, I'd recommend using a 2D axisymmetric model first. This can be generated relatively quickly from your existing 3D geometry. Using a 2D approach means you can assess the sensitivity of the results to changing various factors, such as element types, friction,etc. and also get results in a matter of minutes. Then try running the full kit and caboodle 3D model.
- Thread starter
- #11
I did an axisymmetric analysis. But when ı tried to load a force then error occured. It said Too many attempt for this increament. And axisymmetric cannot solve my problem because after i did this analysis i tried to show fracture area with element deletion. And also I tried deep drawing a square box today with explicit. Its results are true and it is consistent with ABAQUS example problem's results. Cant you suggest any solution about 3D solution.
- Thread starter
- #13
I did a simulation with ABAQUS/Standard but nothing changed. It showed reaction force nearly 5.5 kN again. And also displacement is wrong. Because my experimental displacement nearly 8.2 mm and reaction force 9 kN. There is something wrong but ı couldnt find where. In addition i did axisymmetric analysis clearly. But this time reaction force is 20 kN.
- Thread starter
- #14
I forgot to say that in axisymmetric simulation force is true. Because where displacement is nearly 8 mm, the force is 9.5 kN. But my blank fractured at 15 mm in analysis. Maybe my material data is not true at this point. But again and again the axissymmetric BC cannot solve my problem.
Whether you do the analysis in standard or explicit, the fact that you have quarter symmetry means that your total force needs to be 4 times the force from the model. In an axisymmetric model the total force will be just the force from the model. In my axisymmetric model I got nearly 13kN as a total force with frictionless contact using the displacement you prescribed to the punch. With friction of 0.2 then this increases to just under 16kN, which agrees with your model that produced 4 x 4kN force. Clearly changing the value of friction has some effect on the calculated force. Applying rough friction will give you the worst case. Attached is a picture showing total force against displacement for the friction = 0.2 case, which you can compare with your experimental results.
- Thread starter
- #16
I just modelled 60x60 mm2 which means not quarter, and it have 24 kN max force and 0.25 friction. Can you send me your model? I forgot to say ı changed the material properties to stainless steel. And i use true stress-true strain curves. Is it true for plastic? My force displacement graph is below. And its for 15 mm displacement. After 15 mm it raise a little bit and then down.
I'm glad to see your results now appear more realistic and presumably show better agreement with your measured results. If you want to check that you have plasticity then plot PEEQ, or alternatively add an extra step where you remove the punch and the blank will hopefully not spring back.
- Thread starter
- #18
I'm a little confused as your previous post shows measured forces up to about 18 kN and now you say it fails at 9 kN. I don't know if this is because you've changed the material in the experiment.
In the axisymmetric model, which includes the actual thickness of the blank, the plate thickness reduces considerably at one point and presumably that must be the point of failure. Perhaps if you change your elements for the blank to 3D brick elements then you'd see the same effect. Presumably the material will fail once it reaches UTS for that large strain. You'll need about 6 elements through the thickness to model this if you're using linear elements. I'd also go back to the quarter symmetry model if you want the model to run in less than a day for a dynamic explicit analysis.
In the axisymmetric model, which includes the actual thickness of the blank, the plate thickness reduces considerably at one point and presumably that must be the point of failure. Perhaps if you change your elements for the blank to 3D brick elements then you'd see the same effect. Presumably the material will fail once it reaches UTS for that large strain. You'll need about 6 elements through the thickness to model this if you're using linear elements. I'd also go back to the quarter symmetry model if you want the model to run in less than a day for a dynamic explicit analysis.
- Thread starter
- #20
Ohh there is a little misunderstand. There were 2 Curves. One of them which is higher is duplex Stainless steel and the other lower one is only Stainless steel and my analysis material properties are Stainless steel. and i think the fracture should occurs When i use FLD failure.
- Status