August 3, 2018 at 1:44 pmAdisaSubscriber
I am trying to do analysis from the first post, the analysis must be with solid elements, the analysis is inserting of the pin into the hole. I type to do with more accurately, with less penetration between two parts or the smallest value with is possible. The diameter of pin is 0,1 mm the bigger then the diameter of hole. I need to do with solid elements not with shell.
All the best.
August 3, 2018 at 1:46 pmSandeep MedikondaAnsys Employee
Adisa, The previous topic was already marked as solved, so I've moved this to new post to get you faster help. In the future, please create a new post and provide a link to the next post.
August 3, 2018 at 2:04 pmSandeep MedikondaAnsys Employee
Coming to your question, It looks like Peter already has offered many valuable suggestions and doesn't recommend using shell elements. Have you set up the model already? Are you getting any specific errors? Please post snapshots if you can?
August 3, 2018 at 2:43 pmAdisaSubscriber
Sandeep, I put the example of this type of analysis (inserting pin throught hole), but I need to do analysis of complex construction which is not symmetry, a cross section of complex part is not equal on each tooth of axle.
Thanks in advance
August 3, 2018 at 8:57 pmpeteroznewmanSubscriber
I looked at your knurled metal pin that you want to insert into a plastic hole.
It has a "cap" surface that is not easily manufactured, and that cap will affect how the plastic will flow as the pin is inserted into the hole.
If I make a 45 degree chamfer on the end of the pin, I can remove the cap. This will be make it easier to insert the pin in the hole.
Do you really want that cap, or do you want a chamfer on the knurl?
Also, you will get two different patterns of deformation in the plastic hole depending on whether you push the pin straight in, or if you screw it in. What do you intend to simulate?
August 4, 2018 at 12:33 pmAdisaSubscriber
Peter, I want a chamfer on the knurl and push the pin straight in.
AND I need to determine whether the plastic part cracks and how long the crack will be.
August 5, 2018 at 1:46 ampeteroznewmanSubscriber
The plastic part is not concentric about the pin. Has a circular "plug" been cut out of a much larger part to provide some geometry for this analysis? If so, is the diameter of the cut, and its location somewhat arbitrary? Or is the plastic part an actual complete part?
To make a much smaller and simpler model, assume that the plastic part is symmetrical for an initial model. Then take a small slice of the pin and plastic and use symmetry planes to model that small slice. In the image below, I slice at the peaks, you could slice at the troughs if you prefer. I also cut a big hole in the steel pin since it is much stiffer than the plastic. You could have a zero radial displacement BC that replaces the metal in the center if it deforms too much.
Below is what that slice looks like.
But if you look at a close up of knurled metal parts, they don't have sharp tips. I recommend you add a blend to the tip of each pyramid.
What material properties do you have for the plastic?
This problem is going to be extremely difficult to simulate.
August 5, 2018 at 4:28 am
August 5, 2018 at 9:05 amAdisaSubscriber
peter, plastic part is not symmetry, and is not concentric about the pin. Can I use whole the pin for this analysis, because this plastic part is just part of the complex construction which is not symmetry.
Properties of material:
August 5, 2018 at 11:18 ampeteroznewmanSubscriber
I found a good article on four ways to insert a knurled metal pin into a plastic part. It is for hollow metal pins that are threaded on the inside, but the methods apply to what you have. Two of them involved heat and/or ultrasound to melt the plastic during the insertion. If you go with a melting plastic method, there is no risk of cracking the plastic. One of them is to insert the metal into the mold and flow the plastic around the metal. The fourth is a cold press, which is what you are suggesting.
You say the goal of the analysis is to predict if the plastic part will crack. Has a circular "plug" been cut out of a much larger part to provide some geometry for this analysis or is the geometry an actual complete part? If the geometry of the plastic is larger, please show more of the plastic part as you have cut it too close to the hole for an accurate analysis.
Also, please follow the method on this post to create a spreadsheet to compute True Stress and True Strain for a multilinear kinematic hardening plasticity material model from the 23 C temperature Engineering Stress-Strain curve for your chosen material, which I downloaded from Campus and attached in the zip file below.
August 5, 2018 at 6:27 pmAdisaSubscriber
Thanks Peter for tips.
The anlysis is cold press from video, and I do not change it.
My goal was to show part of the whole analysis on this community, because that the analysis the faster finish, and after that I will apply it advice for all plastic part. My ploblem is that plastic part is not symmetry because that I can not use slice one tooth. I did not convert to true, I use eng. date.
My ploblem is that the solver can not converge, when the pin goes through plastic construction .
I need to use cut out plastic part and use all teeth, and after I do on this part analysis, I will include all plastic part. I do this that lessen calculation time, but I need Tips how to do goes pin though part of plastic construction.
August 6, 2018 at 3:41 ampeteroznewmanSubscriber
If you use Multilinear Plasticity, you must convert from Engineering Stress to True Stress. You said you did not. Please show the material model you are using.
I wanted to see how close the hole is to an edge of the part.
If the hole is less than one diameter from an edge of the part, then that edge and the adjacent hole wall can deform outward in a way that the hole wall 90 degrees around cannot. That would make it so you can't use symmetry and the problem would be extremely difficult to simulate. I'm going to assume that this is not the case since you would need a massive cluster of computer cores solving for a week to do the entire pin in a hole near the edge.
If the hole is more than three diameters away from an edge, then the pin entering the hole will behave the same as if the hole were in an infinitely large part. In that case, you can use symmetry to slice one row (or two rows) of teeth because any row (or two rows) is the same as any other row.
So let's consider the symmetric case. Viewed from the hole, there are 44 identical teeth around the circumference of the pin, but every other row has a half pitch lag. Viewed from the side of the pin, a row has a first tooth, then the rest of the teeth in that row. The first tooth will act like a tool and gouge a groove into the plastic. The second, third and all the rest of the teeth will follow in this groove. The groove may spring back slightly after the first tooth passes, so the second tooth will have to push it back out slightly, but not the way the first tooth had to. That is why I recommended a one tooth model. On second thought, a two tooth model would be better.
I recommend you get a small model that solves and teaches you something about your problem. That is much more useful that a big model that will not solve and teaches you nothing about your problem.
August 6, 2018 at 8:33 amAdisaSubscriber
Peter, I attached material file and the used analysis.
The hole is about one diameter from an edge of the part.
August 6, 2018 at 12:55 pmpeteroznewmanSubscriber
I attached my one tooth model that ran for nearly 8 hours on a 12 core computer.
Here is how far it got:
It will need to run for another 48 hours (or more) to make a groove 0.5 mm long. Since I didn't have your material file when I started this analysis, I used an Explicit material: POLYCARB that uses an Equation of State instead of Multilinear Plasticity. I artificially increased the material density by a factor of 100 in order to reduce the solution time, which was in the hundreds of hours without that density change. I could use a factor of 1000 on the material density to reduce solution time even further, but at some point, the artificially increased inertia forces will affect the results and they will no longer accurately represent the real problem.
This model might take less time to run in Static Structural than it is taking in Explicit Dynamics.
Your mesh is too coarse to do these kinds of simulations.
My single (or two) tooth model might be useful to predict the insertion force for the pin. I can take the reaction force for pushing one (or two) tooth and multiply it by 44 to get the whole pin.
You are interested in trying to predict cracking. Something frequently done in engineering analysis is to create a simpler model and predict if that will crack, and if the prediction is that it will not, that means the more complicated model will definitely not crack, since the simpler model was made using conservative assumptions. For example, if you made a smooth solid pin at the same diameter as the tips of the tooth, that would have to stretch the plastic more than it would get stretched by the teeth, which cut grooves to make space the way a smooth pin would not. This is called a conservative model. If it passes, your real geometry is going to pass. Of course, this is only a useful model if the conservative model passes, if it fails, you can't say that the real model will fail since it may not.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.