October 13, 2018 at 2:31 pmzjuv9021Subscriber
I want to first rotate an object 15 degrees (for an example), and then make a displacement/force towards the fixed end but have the entire pipe locked within that 15 degree rotated plane as I displace it towards the fixed support, please see diagram below:
How can I go about doing this exercise in Mechanical for any "X" degree I choose to rotate this pipe?
October 13, 2018 at 2:54 pmzjuv9021Subscriber
Edit, I don't want the entire pipe locked in the new plane, only a certain length.... Would I just have to create an outer tubing that encompasses this pipe and then cut it to the desired shortened length and "lock it"?
October 13, 2018 at 3:03 pmSandeep MedikondaAnsys Employee
Hi Zack, Please see if this post helps.
October 13, 2018 at 3:07 pmpeteroznewmanSubscriber
Create a Remote Point scoped to the end face of a cantilevered beam. Create a displacement, scoped to that remote point and apply a rotation about X to the remote point leaving all others free, and if you have Large Deflection on, you will get a circular looking displacement of the beam. If you also set Z = 0 instead of leaving that free, the end point will move slightly along the Y axis as the tube bends to the applied angle. Do that in step 1 of a two step solution. You can set X=0 if you want or leave it free.
Then in step 2, You can apply a force to the Remote Point in the Y direction and push the end further along the line Z=0, because the displacement in step 2 will holding the angle at the same value as well as hold Z=0.
October 15, 2018 at 1:37 amzjuv9021Subscriber
Thank you. I'm still a little confused.
Please see diagram below of what I would like to achieve:
I would like to ultimately be able to vary the degree and then constrain movement within the bottom layer (pink/salmon colored, frictionless or rigid as I don't care about it's deformation, currently), then apply an axial displacement on the tubing to see the characteristics/behavior that occur within the free movement plane.
I hope this helps clarify. Any input on how to best approach this physical problem is greatly appreciated.
October 15, 2018 at 5:13 ampeteroznewmanSubscriber
One aspect of FEA modeling that may not be obvious to a new user is the idea of of the zero stress state of a part. You show in blue, Axial Displacement #1, with a curved shape that you want to push axially and contact the yellow part. The problem is that the tube started out life as a straight tube. That is the shape it is in when it is manufactured. You have to bend it into the curve shown in blue before you start to push it axially. While you could draw the tube as curved in the CAD system and mesh it and start to push it axially, that simulation would behave differently than a tube that started out straight in a horizontal line, was bent into the curve and then pushed axially. The reason it will behave differently is the state of stress in the tube after it is bent will affect how it deforms when it makes contact with the wall.
You have been drawing straight tubes and trying to bend them, so maybe you already understood this concept.
When you take a straight tube fixed at one end and apply a 90 degree rotation to the other end face, you can get a nice circular shape. There is an APDL command snippet that allows the current position of a specific degree of freedom of a node to be fixed at the current position. That could be used on the end of a straight tube along the X axis after it has been bent into a curve to hold the node fixed in X at whatever value that was, while moving the node in the Y coordinate from wherever it was at the end of step 1.
When you say axial, you mean that it is following the path of the tube in a channel in the salmon part. I can imagine modelling the salmon part as a two-piece rigid form. Initially, the right part with the concave face is retracted way to the right. The left part with a convex face is fixed and the straight blue tube is pulled down to make contact with the left part in step 1. In step 2, the right part of the salmon form is translated to the left into place as shown above. In step 3, the tube is pushed and now has a path to follow, and freedom above the salmon part to deform as it makes contact with the yellow part.
October 15, 2018 at 6:45 pmzjuv9021Subscriber
Could I wrap the salmon part around the tubing, in essence creating an outer tubing wrapped around the manufactured one, rotate the end of the straight tube a fixed degree (e.g. 30 degrees), and then lock the salmon wrapped tubing in my second step and then displace or push my manufactured tubing through this locked tubing path?
October 15, 2018 at 11:31 pmpeteroznewmanSubscriber
Yes, you could have a salmon tube outside the blue tube. You could move the salmon tube into position, carrying the blue tube with it and fix the salmon tube then push the blue tube.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- How to calculate the residual stress on a coating by Vickers indentation?
- 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.