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!
interaction between bolt and hole 1
- Thread starter pouya1983
- Start date
- Thread starter
- #3
Thanks for you message but when we consider surface-to-surface interaction with hard contact in normal behavior after runnig,the program leave with this error:" there are too many attempts with this increment", how can I solve this problem?
Thank you
kind regards
Thank you
kind regards
Does that mean that you can solve the problem when you use tie constraints instead? Tie constraints are linear whereas contact is not, so it is no surprise that it does not converge sometimes. In that case, there are many things to check.
I would start with looking at the Abaqus .msg file to search for clues on why it is not converging (there is a lot of useful information there but it is sometimes hard to decipher). One possibility for example is that the bolt has insufficient boundary condition to eliminate rigid body rotation about itself. In true then friction should help. Another possibility is that there is too much initial penetration between the bolt and hole resulting from coarse elements in that region. In general, Automatic Stabilization helps with contact, and so does using small increment sizes.
I hope this helps.
Nagi Elabbasi
Veryst Engineering
I would start with looking at the Abaqus .msg file to search for clues on why it is not converging (there is a lot of useful information there but it is sometimes hard to decipher). One possibility for example is that the bolt has insufficient boundary condition to eliminate rigid body rotation about itself. In true then friction should help. Another possibility is that there is too much initial penetration between the bolt and hole resulting from coarse elements in that region. In general, Automatic Stabilization helps with contact, and so does using small increment sizes.
I hope this helps.
Nagi Elabbasi
Veryst Engineering
- Thread starter
- #5
thank you for your message
According to manual if the diameter of the bolt and hole are the same we can use constraint contact like tie but if the diameter of bolt is less that the hole we should use interaction like surface-to-surface interaction,am I right?
The bolt tie two segment to each other,I created two partitions on my bolt that each partition is in contact with the hole of each segment and tied the exterior surface of each partition to interior furface of each hole,is it correct?
According to manual if the diameter of the bolt and hole are the same we can use constraint contact like tie but if the diameter of bolt is less that the hole we should use interaction like surface-to-surface interaction,am I right?
The bolt tie two segment to each other,I created two partitions on my bolt that each partition is in contact with the hole of each segment and tied the exterior surface of each partition to interior furface of each hole,is it correct?
The partitioning that you did makes sense and you can use it for both tie constraints and standard contact. I guess you must have also defined contact between the two flat surfaces of the partitions.
I couldn't find the part in the manual that you mentioned for deciding between tie and contact for the bolt. If contact between the bolt shank and the hole is the best option and it's not converging then it's usually better to not have any contact or tie constraints along the bolt shank. The bolt in that case needs to be sufficiently supported at its head and/or nut, and it should mainly be carrying a tensile load (not much bending/shear). Check out Example 1.1.1 in the Abaqus Examples Problems Manual ... that's what they do there.
I'm curious to know how it turns out!
Nagi Elabbasi
Veryst Engineering
I couldn't find the part in the manual that you mentioned for deciding between tie and contact for the bolt. If contact between the bolt shank and the hole is the best option and it's not converging then it's usually better to not have any contact or tie constraints along the bolt shank. The bolt in that case needs to be sufficiently supported at its head and/or nut, and it should mainly be carrying a tensile load (not much bending/shear). Check out Example 1.1.1 in the Abaqus Examples Problems Manual ... that's what they do there.
I'm curious to know how it turns out!
Nagi Elabbasi
Veryst Engineering
- Thread starter
- #7
You're welcome. I looked at the figure and it does not reveal that much so can't find anything more to add. The approaches that we discussed above are good and work in many cases. However, sometimes getting the FE program to converge is tricky.
One more thing that may help is to switch bolt loading from applied bolt tension to bolt shortening. This is like going from force loading to displacement loading ... it is easier to converge.
Good luck.
Nagi Elabbasi
Veryst Engineering
One more thing that may help is to switch bolt loading from applied bolt tension to bolt shortening. This is like going from force loading to displacement loading ... it is easier to converge.
Good luck.
Nagi Elabbasi
Veryst Engineering
- Thread starter
- #9
-
1
- #10
Dear Pouya1983
The answer to your first question depends on the ratio of the bolt diameter to the hole diameter in the physical model. The FEA model should follow the physical model. Why would the bolt diameter be larger than that of the bolt hole?
The CLEARANCE tab is a very useful feature. It may come in handy for your problem. It provides a way to replace gaps/over-closures measured from the finite element mesh with user-defined one. If you have two concentric cylinders (which you do), and let's say there is a geometric gap of X. If you then create an FE mesh and calculate the FE gap you'll see that the values will be way different from X in most cases (due to replacing cylindrical surface with linear/quadratic segments). The CLEARANCE feature offers A way to replace this FE gap with X.
Nagi Elabbasi
The answer to your first question depends on the ratio of the bolt diameter to the hole diameter in the physical model. The FEA model should follow the physical model. Why would the bolt diameter be larger than that of the bolt hole?
The CLEARANCE tab is a very useful feature. It may come in handy for your problem. It provides a way to replace gaps/over-closures measured from the finite element mesh with user-defined one. If you have two concentric cylinders (which you do), and let's say there is a geometric gap of X. If you then create an FE mesh and calculate the FE gap you'll see that the values will be way different from X in most cases (due to replacing cylindrical surface with linear/quadratic segments). The CLEARANCE feature offers A way to replace this FE gap with X.
Nagi Elabbasi
- Status
Similar threads
