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 cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
"Infinity friction" in contacts - When use it?
- Thread starter pio3
- Start date
pio3,
Mechanica WF4 offers the option to enforce "infinite friction" on a contact interface. It also offers the option to create a measure of possible slippage, based on a friction factor you input.
Mechanica does NOT have the option to calculate the scenario where the item is loaded to the point of impending slip and then the dynamic friction factor kicks in while the part slides.
As such, if you think your parts are going to act together via friction during the static load, use infinite friction to assess the load distribution in the parts. The slippage measure will give you an indication if tangential loads exceed the frictional resistance, and you can assess if a more detailed analysis is needed. If you need to accurately know stresses in the region of contact, you can either define a tight mesh in that region or turn on "Localized Mesh Refinement" in the "Convergence" tab (this will take longer to run).
One other note: if you don't use infinite friction, you may have to add additional constraints to prevent the part from flying away in the tangential direction.
Mechanica WF4 offers the option to enforce "infinite friction" on a contact interface. It also offers the option to create a measure of possible slippage, based on a friction factor you input.
Mechanica does NOT have the option to calculate the scenario where the item is loaded to the point of impending slip and then the dynamic friction factor kicks in while the part slides.
As such, if you think your parts are going to act together via friction during the static load, use infinite friction to assess the load distribution in the parts. The slippage measure will give you an indication if tangential loads exceed the frictional resistance, and you can assess if a more detailed analysis is needed. If you need to accurately know stresses in the region of contact, you can either define a tight mesh in that region or turn on "Localized Mesh Refinement" in the "Convergence" tab (this will take longer to run).
One other note: if you don't use infinite friction, you may have to add additional constraints to prevent the part from flying away in the tangential direction.
- Thread starter
- #3
- Thread starter
- #4
Ok, so now the question:
as u can see in the attached example I have two plastic components that are in interference in a drawing condition (when they are assembled in ProE of course).
In reality the 2 components are in contact, and the orange one is able to slide along the green one (but normally is blocked in the upper part).
I applied a force against the orange one (simulating a spring), and i want to see if this force is able to detach the contact between the 2 components.
As you can see in the left picture, analysis is made without "infinity friction" and the orange component "fly away" from the green one.
In the right picture the same analysis but with "infinity friction" applied. As you can see we have kept the contact.
So the 2 behaviors are different.
Now, i don't know if in reality the force is able to detach one component from the other. How can I decide if I have to use "infinity friction" or not??
Thanks a lot
as u can see in the attached example I have two plastic components that are in interference in a drawing condition (when they are assembled in ProE of course).
In reality the 2 components are in contact, and the orange one is able to slide along the green one (but normally is blocked in the upper part).
I applied a force against the orange one (simulating a spring), and i want to see if this force is able to detach the contact between the 2 components.
As you can see in the left picture, analysis is made without "infinity friction" and the orange component "fly away" from the green one.
In the right picture the same analysis but with "infinity friction" applied. As you can see we have kept the contact.
So the 2 behaviors are different.
Now, i don't know if in reality the force is able to detach one component from the other. How can I decide if I have to use "infinity friction" or not??
Thanks a lot
- Thread starter
- #5
pio3,
One question about your sketched constraints: Does the orange part have a displacement constraint in the vertical direction (as shown in your hand sketch), or is it only on the green piece? If both parts are constrained, this could affect your assessment of the holding power of this interference feature.
With regard to friction, it looks to me like you want to be using Infinite Friction for your analysis. To be certain, you should make sure you have enabled the 'slippage indicator' measure in your contact definition. Here are the steps:
1) Insert -> Connection -> Interface
2) In dialog box, Dropdown menu 'Type' = "Contact"
3) Properties:
x Infinite Friction
x Create Slippage Indicators
Coefficient of Friction for Slippage Indicators = (Fill in your number here)
In your Report file (*.rpt), you can look at this measure to determine if the part 'would have' slipped for this coefficient of friction. If the slippage indicator value is positive, then your part may have slipped.
Let me know what you find.
Peter
One question about your sketched constraints: Does the orange part have a displacement constraint in the vertical direction (as shown in your hand sketch), or is it only on the green piece? If both parts are constrained, this could affect your assessment of the holding power of this interference feature.
With regard to friction, it looks to me like you want to be using Infinite Friction for your analysis. To be certain, you should make sure you have enabled the 'slippage indicator' measure in your contact definition. Here are the steps:
1) Insert -> Connection -> Interface
2) In dialog box, Dropdown menu 'Type' = "Contact"
3) Properties:
x Infinite Friction
x Create Slippage Indicators
Coefficient of Friction for Slippage Indicators = (Fill in your number here)
In your Report file (*.rpt), you can look at this measure to determine if the part 'would have' slipped for this coefficient of friction. If the slippage indicator value is positive, then your part may have slipped.
Let me know what you find.
Peter
- Thread starter
- #7
Hello Peter,
yes, there are constraints on both components in all direction in the upper part. This because the 2 components are fixed inside an other assembly (that I have suppressed for the analysis).
How can I fill the "Coefficient of Friction for Slippage Indicators"? Do you think I have to find the number by a sperimental test?
For a better explanation of the last image i've attached, in both cases there is a contact, but in the second one I have activated only "infinite friction" (not "Create Slippage Indicators" beacuse I don't know wath number I have to use).
Waiting for your impression..
Pietro
(I'm italian, so I'm Peter as you if you want to translate in english.. :-D). And sorry for my not good english.
yes, there are constraints on both components in all direction in the upper part. This because the 2 components are fixed inside an other assembly (that I have suppressed for the analysis).
How can I fill the "Coefficient of Friction for Slippage Indicators"? Do you think I have to find the number by a sperimental test?
For a better explanation of the last image i've attached, in both cases there is a contact, but in the second one I have activated only "infinite friction" (not "Create Slippage Indicators" beacuse I don't know wath number I have to use).
Waiting for your impression..
Pietro
(I'm italian, so I'm Peter as you if you want to translate in english.. :-D). And sorry for my not good english.
Pietro,
Pleased to meet you!
Not knowing what your materials are, I'd think you could do a quick google search for the coefficient for your material pair. For lack of anything better, Machinery's Handbook cites a range for coefficient of friction for a Nylon-Nylon interface as 0.15 - 0.25
If this is a safety or performance critical feature, you might eventually want to do some experimental testing on the friction, but for your initial analysis, I'd try a book value. (Also, keep in mind that, whatever number you choose to put in the Slippage Indicator box, Mechanica will still apply infinite friction. So, your value will NOT change the analysis results for displacement and stress.)
Good luck,
Peter
Pleased to meet you!
Not knowing what your materials are, I'd think you could do a quick google search for the coefficient for your material pair. For lack of anything better, Machinery's Handbook cites a range for coefficient of friction for a Nylon-Nylon interface as 0.15 - 0.25
If this is a safety or performance critical feature, you might eventually want to do some experimental testing on the friction, but for your initial analysis, I'd try a book value. (Also, keep in mind that, whatever number you choose to put in the Slippage Indicator box, Mechanica will still apply infinite friction. So, your value will NOT change the analysis results for displacement and stress.)
Good luck,
Peter
- Thread starter
- #9
MarkCopland
Mechanical
Hello, Pio3 and Petiesmo.
I got two different points regarding with the FEA analysis that Pio3 is doing.
Regarding with the fea analysis in plastic like material, please have a look at the thread “ Pro/mechanica and plastic like materials”, so we don’t mix opinion in this thread.
Now regarding with the contact analysis in pro/mechanica:
Does Mechanical calculate dynamic friction interaction?. (I don’t have the dynamic add MDO, until I know MDO perform dynamic friction interaction).
If is it not, I guest that mechanical can only calculate static “interaction” between two (or more) solids (as example: to use contact to simulate in a”more” accurate way the force transmission between two solids), so it can give you an accurate contact pressure force and contact area (hertzian contact).
1) So, How can you calculate if this force if going to detach the contact?.. ( with the Slippage Indicators?.)
2) if is like that, I will take your model and unconstraint the orange part (leaving only the constrain in the green part), tick infinite friction and have a look in the results.
I got two different points regarding with the FEA analysis that Pio3 is doing.
Regarding with the fea analysis in plastic like material, please have a look at the thread “ Pro/mechanica and plastic like materials”, so we don’t mix opinion in this thread.
Now regarding with the contact analysis in pro/mechanica:
Does Mechanical calculate dynamic friction interaction?. (I don’t have the dynamic add MDO, until I know MDO perform dynamic friction interaction).
If is it not, I guest that mechanical can only calculate static “interaction” between two (or more) solids (as example: to use contact to simulate in a”more” accurate way the force transmission between two solids), so it can give you an accurate contact pressure force and contact area (hertzian contact).
1) So, How can you calculate if this force if going to detach the contact?.. ( with the Slippage Indicators?.)
2) if is like that, I will take your model and unconstraint the orange part (leaving only the constrain in the green part), tick infinite friction and have a look in the results.
- Thread starter
- #11
Hi MarkCopland,
I found something inetresting.
Have a look to this link:
Bye
Pio3
I found something inetresting.
Have a look to this link:
Bye
Pio3
- Status
Similar threads
- Locked
- Question
- Locked
- Question