Learning Forum

[5802lucky]

sir i hided the pinion and gear separately and saw the stress generation the stress was concentrated at the centre i.e the middle portion

I  applied face meshing with everything fine i.e span centre and everything fine and smoothing high and high relevance at the contact region including both tooth and tooth space of pinion and gear i.e nearly  20 and 30 faces respectively  then i got these results

SIR I JUST WANT TO KNOW ARE THE RESULTS CORRECT SO THAT I CAN PUT THESE DATA IN MY REPORT AND PRESENTATION OR I HAVE TO APPLY SOME CHANGES

(off topic-sir regarding that faulty file i am working on that i will post with archieved file from now on very soon,i was trying to delete the messeage but whole conversations got deleted)

THE  face meshing i applied the details are here below

sir are these okay or if i apply more moment the will i get better stress deformation that will be visible well?

SIR ANY SUGGESTION?

 

[peteroznewman]

As I said in the deleted discussions, you must do a Mesh Refinement Study.

Make a plot that looks like the one shown below for each gear, then you can be confident that you have a proper mesh.

[5802lucky]

thank you sir but how to find that max stress and element size graph in ansys .What is the procedure? where is that option?Do i have to study the whole ASME V&V10.1 

[peteroznewman]

Maximum stress is on the legend.

Element size is in the Sizing Mesh Control

No, you don't need to read the ASME V&V10.1 guidance.

[5802lucky]

thank you  sir i will try with this i hope in this i will get nearly correct results

Now sir i have been told to get the response at varying load under specific frequencies .I have done modal analysis of helical,herringbone and crossed helical gear pinion assemblies.I have kept the number of modes as 10 as told and have gotten different natural frequency wrt modes in total deformations.

Sir now what to do in harmonic analysis,What should be my boundary conditions and load criteria.I have not been told in details about this.Should i just apply the same boundary conditions and moment as applied in static and transient or i have to apply by rotational velocity? I have watched some youtube videoes regarding this ,they soonafter modal analysis jump to harmonic analysis with copying the same model as modal analysis and then applied same boundary conditions and load  as static structural .Then what is the need of copying the total deformations of modal analysis to harmonic analysis? What exactly is the reasons of it?

Then to perform this should i have to do it in explicit also? or harmonic is sufficient in my context

[5802lucky]

sir please give me ideas regarding the boundary conditions and load application of above mentioned

[peteroznewman]

What is on the other end of the shaft that has the gear?  How long is the gear shaft?  What is the gear shaft diameter? Where are there bearings?

What is on the other end of the shaft that has the pinion? How long is the pinion shaft? What is the pinion shaft diameter? Where are there bearings?

A Modal analysis is done on the system that includes the shafts, bearings and the gears.

[5802lucky]

but sir i have not been told to design shaft and bearing ,only to get the response under varying load under specific frequencies

i have kept the shaft diameter as 1/4 th of pitch circle diameter as advised. Can it be done by only applying shaft not bearing, because i have not given any clue about bearings

FOR MODAL ANALYSIS IS IT NECESSARY TO HAVE A GEARBOX? DO I HAVE TO MAKE A WHOLE GEARBOX FOR IT?

[peteroznewman]

Let's assume there is a bearing on the shaft close to the gear and the shaft is 200 mm long. Assume the same on the other side of the mesh for the pinion. The first natural frequency of that system is probably the shaft twisting and the gear and pinion rotating against each other with the teeth in mesh. Now make the shafts 300 mm long, the first natural frequency goes lower, or reduce the shaft length to 100 mm and the twisting mode natural frequency goes higher, but maybe that is no longer the first natural frequency. Do you see that you need to look at the system and not just the gear and pinion?

[5802lucky]

so sir is modal analysis possible without bearing? only taking shafts with variation in length?

 

[5802lucky]

And sir the rotational velocity option in load is applied on full body only.Will that give correct result in context of gear drive if remote displacement is applied in right dof for static analaysis?

[peteroznewman]

No, without the bearings the gear and pinion will flop about all over the place. The bearings are a required element of the system.  You don't need to model the bearing itself, just make a separate face on each shaft the width of the bearing, then use a Remote Displacement on that face. That way you can hold lateral displacements to zero, leaving all other directions and rotations free.

What is the rotational velocity?  It is probably small enough to have a negligible effect. We are not talking about gas turbine rotational speeds here are we?

[5802lucky]

no sir i applied same torque i.e  in crossed helical and parallel helical gears, so the stress was higher in crossed helical ,it was acceptable because in crossed helical, there was point contact or line contact and due to the angle ,the faces in contact was 4 only ,where as in parallel shaft axis helical gear there was area contact and also the faces in contact was 5 (Both parallel and crossed helical gear-pinion assembly had same dimension only alignment was different)

BUT  when i applied  a moment of 6000 rpm i.e 628.32 rad/sec in pinion of both parallel helical gear and crossed helical gear ,this time the result was opposite.This time with the same rotational velocity applied to the pinion body, the result reversed i.e the stress i.e max equivalent stress was higher in parallel helical gear instead of crossed helical gear

SO  is in my context , rotational velocity applying to whole pinion body is correct procedure to compare stress?

[peteroznewman]

Please show your mesh refinement study plot and a close up image of the elements on the teeth for the smallest element size on the plot. Did you figure out how to plot the stress on just one body (without making the other body hidden)?

[5802lucky]

sir whenever i activate advanced sizing option on in mesh to kkep everything fine then my computer hangs, so i take coarse but i perform refinement with factor 3 on  all the contact tooth and some tooth around with face meshing.Sir i think the mesh refinement study plot is to be plotted by excel manually , you showd me where is the size of element but did not show me if there is any option in ansys to show the plot. So i ignored the plot , i think it will be done in excel i  will perform and show it to you.

[peteroznewman]

Don't use advanced sizing option. Use uniform sizing option with a coarse mesh size and a face sizing mesh control as I showed above.  Take the number used in the face sizing mesh control and the maximum from the stress plot and type those into Excel to make the plot.

[5802lucky]

sir there is no advanced option in face sizing details i have taken 5 mm is it okay. i took everything coarse and i also took refining 1 in the contact area along with this element size. 5 mm and face meshing in cont area also

this is my conditions at cont area keeping other coarse

 

[5802lucky]

here i have taken element size from 0.5 to 5 and similarly stresses from maximum to minimum respectively i.e 10 datas in each axis

In below i have taken from 0.025 to serially 10 value i.e 0.225 in x axis to stress from higher to lower

[5802lucky]

sir when i was doing that refinement with 3 factor it was taking huge amount of time and stress was coming higher, but after taking element size from  default to 5 mm and reducing refinement to 1 , it was solved within very few minute.So as only refinement with factor 3 alone takes huge time to solve can i assume that this gives the best nearabout result? In refinement 3 alone the stress was almost double than i got in refinement 1 anf face sizing of 5 mm .In refinement 3 alone the stress was 6e7 almost, now in refinement and element size 5mm stress max is 3.6e7 and iin only refinement 1 the stress was almost 2e7

And sir another question-If i will slice both gear and pinion ,is it necessary to slice in same angle ? If i will slice gear and pinion randomly at different angle it will save time ,but will it give wrong results?

[peteroznewman]

Yes, these mesh studies take a long time.

Don't use Refinement.

Plot the individual points of stress for each Face Element Size.

You can have a narrow angle for the gear and a wide angle for the pinion. Try to keep the circumferential length of each about equal.

[5802lucky]

Sir was my previous plot wrong?i made couple of plots as i was not sure. there are ten values of stress from minimum to maximum and the element size is 5mm i.e 0.005 m so in x axis what should be my range at what intervals .I  kept all the values from maximum to minimum in y axis serially fro bottom to top.Is it the right procedure?

sir its okay if refinement with factor 3 tkes huge time , but will it give closely perfect results? Then its okay

[peteroznewman]

My plot shows individual points.

Your plot has no points visible. Just a line. Where are the points?

A good interval between points on the element size axis have a constant factor of 1.5

[5802lucky]

1.5 mm? IN MY X AXIS I WILL START FROM 0, 1.5, 3,4.5 etc?? but there are 10 values in legends coloumn of stress so i will put those and in my x axis if i start from 0 and take increment of 1.5 then it will exceed 5, but my element size that i have taken is 5 mm

in y axis stress is in pa , so in my system the element size i have given is 0.005 m

but in your plot interval is 0.025mm it has started from 0 to 0.175 

Should i also take those x axis data?

but sir your have plotted by taking 7 data  in each axis , but if i want to show all the 10 minimum to maximum stress values, from where should i start my x axis point with exactly what increment , am little confused

[peteroznewman]

Below is a list of numbers, starting at 3 mm, where each subsequent row is the row above divided by 1.5 and the result rounded off to 3 digits.

• 3.000


• 2.000


• 1.333


• 0.889


• 0.593


• 0.395


• 0.263


• 0.176


• 0.117


• 0.078


• 0.052


• 0.035


• 0.023

You can compute the maximum stress for each row and plot that on an X axis that goes from 0 to 3 mm.

[5802lucky]

so individually i have to simulate for these element size one by one

sir another question when you told to keep the gear fixed and the pinion in revolute joint ,  the revolute joint has? to be selected from body to ground coloumn or body to body coloumn?

And sir in pin ball region in contact portion .the radius of less than twice of face width is okay? Does specifying pinball region radius in frictional contact affect the results 

[peteroznewman]

You can use Workbench Parameters and the Parameter Set worksheet to fully automate the generation of this table of values.  The Element Size in the Mesh control becomes an input parameter and the Maximum Stress becomes an output parameter. 

The revolute is Body-Ground.

You can leave the Pinball Radius Program Controlled when the faces are touching in CAD.

[5802lucky]

okay sir,thank you, but  i have taken the pin ball region radius 7e-002m where my facewidth contact zone of gears is 100mm. Is this wrong? will this type of specifying pinball radius affects results or give inappropriate results?

[5802lucky]

sir in crossed helical system only the pinion disappears in results of stress when pinball region i make program controlled

Then when i take pinball radius 7e-002m then pinion does not disappear,but the stress result i.e equivalent stress reduces to almost half, earlier you sent me a photo of analysis settings of static structural to prevent the pinion diappearing when clicking results, but that did not work.So i kept the pinball radius manually  then the disappearance problem gone

but today as i did again with pinball radius program controlled on the stress came twice that of the pinball radius 7e-002m (the moment applied was same)although pinion was disappearing

[5802lucky]

sir any suggestion? although in one of my model little penetration is there still in program controlled its showing error about CONT , FAR OPEN ,although adjust to touch option is also checked.

so i make the pinball radios 7e-002. What is the criteria for the value of radius of pinball

in my case there is penetration then also its showing no contact found in case of program controlled. What is the solution?.Bellow i have given some photos of penetration and pinball 

[5802lucky]

is this 7e-002 m radius pinball is correct step for it? although as in upper photos you can see penetration are there still error of no contact found comes in program controlled but in this 7e-002 m radius pinball region definition results came but is it valid?

 

[peteroznewman]

Read ANSYS Help on Contact for the use of pinball radius.  I don't have 16.2 on this computer so I can't give you exact instructions.