Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
When two or more bodies are brought from CAD into the FEA software, the FEA program is able to interpret that there’s multiple bodies but makes no presumption about what the relationship of these bodies are as far as relative motion is concerned.
Are the bodies completely joined to one another (such as with a full penetration weld), are they able to slide relative to one another, or maybe they are restricted from sliding – but readily able to pull apart? Defining these relationships, how the parts may move (or not be able to move) relative to one another, is what the various contact types allow us to define.
There are several contact types available to represent how your model interacts in the physical world. You should aim to apply what is needed to represent actual conditions as best as possible (similar to constraining a model).
There will be some variability, depending on the specific finite element analysis package you are utilizing, but you should generally expect to find contact types that will fit your structural analysis. Below, note what Inventor Nastran includes and when you might utilize each type:
The settings for manual and automatic contact sets can be modified. The dialog box allows users to change the participating entities, contact type, stiffness, friction, and more.
Contact allows analysts to more precisely model the interactions between parts. However, keep in mind that adding contact to a model will increase solution time. We will examine two reasons for this.
Applying contacts in an analysis will lengthen the solution time by some amount. This is not reason to not utilize contact, but rather, information to know to allow ahead of time for longer solution times and for consideration of where and when to utilize contact.
Given the illustration of these simple block examples, it is possible to see how the effects can be even more extreme with a large assembly of many parts. If a goal is to try and keep solution time to a minimum, there are a few different techniques – you might be able to utilize one or more.
Thinking through the model before diving into the analysis, such that contact is utilized only when and where required, can help save significant solution time.
Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
00:08
In this demonstration, I will be covering contacts within Inventor Nastran,
00:12
as well as going through where they're best used and the settings involved with each type.
00:19
So, for this example, I'll be using this hitch assembly again here.
00:22
And taking a look at it, you can see that there are four individual parts or four individual bodies that have been modeled in the assembly.
00:29
So, if I go over to the model tree, you'll see those four-part files, you'll also see that relationships have been created.
00:37
So, these mates that have been added in within the assembly environment do not transfer to the FEA environment or Inventor Nastran.
00:46
So, I need to provide Inventor Nastran with information on how these individual parts interact with one another,
00:53
and what surfaces may come into contact or are welded or bolted together.
00:60
So, to do that with Inventor Nastran, I need to create what are called contacts or contact sets between each of those surfaces.
01:07
So, you'll see contacts is up on the ribbon here right next to setup and next to mesh settings.
01:13
If I do not activate any contacts and I select "Run", what you'll notice is it kicks off like a normal linear static analysis.
01:21
Everything looks Ok.
01:24
But then you'll get this E5000 series error.
01:27
So, if you ever get an E5000 or an E5004, double check that you have contacts applied and that these settings are correct.
01:36
If you do not have contact created, that means there's some level of instability or a singularity that's been detected.
01:42
So, what's really happening is this ball right here is getting pulled off into infinity,
01:47
the parts are separating and the solver is not able to calculate the stiffness of those interactions.
01:53
And so, it fails.
01:55
So, what we'll do is we'll add contacts to fix that problem.
02:01
So, I'll walk you through the two primary contact types, automatic and manual.
02:06
So, the way that automatic contact works is it uses a predetermined default tolerance range.
02:13
Any surfaces that fall within that range will be given a default contact type, which is typically bonded.
02:20
Now to find where that's at, you actually have to edit the analysis.
02:25
So, I'll right click and edit and then I'll go into the options tab right here and you'll see Contact data, Contact type is Bonded, Tolerance 0.0039.
02:37
This value is essentially 0.1 millimeters, but in inches, it's 0.00393.
02:44
And the contact type of bonded is what will be applied.
02:47
So, what this means is any surface of separate parts that are within 0.0039 will be assigned a bonded contact upon running auto contacts.
03:00
This works really well when you have a few parts that are relatively close to one another,
03:05
and you know, are going to be bonded, you can go back later and change them from bonded with separation.
03:11
This is a really good way to start because it'll make sure that things are held together.
03:15
And then you can work backwards, gradually releasing the degrees of freedom and allowing things to separate or slide as you go.
03:23
So, what I might do is leave the default contact tolerance as it is and just go ahead and run it to see what I get.
03:30
So, I'll select "Auto", it's going to detect contacts within that range.
03:36
And now there's a Surface Contacts folder that's been created in the analysis tree.
03:40
If I expand it, you'll see there's been 14 contacts created.
03:44
If you click on them, it'll show you the two faces that are in that set,
03:49
which in this case is the hitch to the receiver that has several faces on it.
03:54
Which means if I highlight that whole set of eight,
03:58
it's essentially the eight surfaces going around the outside of the hitch touching where it comes into the receiver.
04:07
The next set here is between the pin and the receiver, which is essentially going to be both sides where it passes through those holes.
04:16
I also have the hitch to the pin, pin to the receiver there on that side,
04:22
the chrome ball here where it is welded to the hitch and then the hitch to the pin on the other side.
04:28
So, what it's doing is it's going through and identifying all of those surfaces.
04:34
So, if you want to identify what this creates and what the result would be,
04:39
I recommend running it at least once to understand the effect of these bonded contacts on the stiffness,
04:46
and the ultimate result of this analysis.
04:48
So, I'll go ahead and select "Run" and this should eliminate that E5000 series error that I was getting.
04:55
I have a constraint, a load and now bonded contacts between all of the faces.
05:00
So, it should be a stable model.
05:04
So, I'll select "Ok".
05:06
And I should see this kind of bend downwards, create some stress on that filet there near the weld, about 10,000 psi of stress.
05:14
Everything up here is mostly rigid near the constraint.
05:17
And this pin and receiver is behaving very stiff.
05:22
And this is an area where maybe I consider switching from bonded to separation.
05:27
The issue with a bonded contact here is it's creating a welded connection where maybe I want to allow some level of sliding or opening.
05:35
So, we'll break down the contact types here and make a couple of changes in that region to potentially generate a better result.
05:43
So, I'll go ahead and unload these results and walk you through the different contact types before we make any changes.
05:49
So, if I go to manual contacts, you will see the contact type here.
05:55
There's a drop-down menu and there are a total of eight different contacts.
06:01
The most commonly used contacts are going to be your separation and your bonded.
06:04
Separation is going to allow the two surfaces to slide and rotate and separate from one another.
06:11
The only thing it does is it prevents surfaces from passing through one another.
06:17
So, just like if you were to put your pencil down on the desk in front of you, it can't pass through that surface.
06:23
That is a separation contact that has been generated.
06:26
Bonded contacts are essentially a weld that joins two surfaces together.
06:32
It connects the translational degrees of freedom of those nodes.
06:36
Sliding, no separation allows for sliding between parts, but they cannot separate intention or compression.
06:43
They can just slide in plain.
06:44
This is great for pinned connections.
06:47
Separation, no sliding can only be used in a nonlinear analysis.
06:51
And this is essentially infinite friction.
06:54
Offset bonded is great when you have two shell elements that have rotational degrees of freedom being bonded together.
07:01
So, shell to shell, shell to solid interactions or anywhere you have a fairly significant gap between surfaces.
07:10
Offset bonded is going to be a little bit more rigid and reliable than a traditional bonded contact.
07:16
But it's still considered a weld.
07:19
You also have shrink fit sliding and shrink fit no sliding.
07:21
These can only be used in nonlinear analysis when you have interference from a shrink fit.
07:27
And then you can also just disable the contact as well if you'd like to keep it in the list, but turn it off.
07:37
So, jumping back to the contacts in the list here,
07:42
I may change some of these to allow a little bit more realistic interaction between the parts where I have the pin coming through.
07:50
It's not being welded through the receiver.
07:53
The hitch is also not going to be welded to the receiver.
07:57
Those are free to slide, rotate and separate.
08:02
So, I want to change those to separation.
08:05
However, the hitch ball will be welded to the hitch at the end here.
08:11
So, that area I may leave as bonded because it will be welded in that region.
08:17
So, if I go ahead and I select all of these contacts here, I can go ahead and edit.
08:24
And notice when you do a group select, you can't change the entities that are involved or the name.
08:31
But what you can do is you can change the contact type here to separation and then select "Ok".
08:37
And you'll notice the icon changes from two blocks together to two that are offset and separated.
08:43
That is the icon you'd like to see there for separation.
08:47
So, that's been updated, I can then go through and update some of these other contacts as well if I'd like to.
08:52
But I'm going to leave, you know, potentially that chrome bone and hitch the same.
08:56
So, I might edit some of these other contacts here, make those separation as well.
09:04
So, that means a lot of things are able to separate and slide.
09:08
But ultimately, the weld here will keep this whole thing intact.
09:15
Now, when I solve this, because I'm allowing for more sliding and degrees of freedom, it will take longer to solve than a fully bonded model.
09:24
So, I'll select "Run" and then I'll come back and view the results when it's done.
09:30
So, after it solves, you'll see the result looks quite different.
09:33
I still have a very similar maximum stress in this area here near the hitch ball in the weld.
09:39
But notice, there's a little bit more bending sliding and then stress being applied here,
09:45
to where that pin is going to interact with the hitch receiver and the internal hitch there, which is what I would expect.
09:53
I'd expect there to be some pressure there where the load is transferred,
09:57
and some pressure here where it starts to bend before this whole area up here was blue because it was too rigid.
10:05
It was as though the entire surface was welded.
10:08
When in reality, those two surfaces can slide freely and the pin should be taking the majority of that sheer force due to the hitch ball.
10:18
So, I'm satisfied with that result, I can then go ahead and save my study.
10:22
And then from here you would continue on running a convergence analysis on the mesh and then you'd be ready to use that result for design purposes.
10:34
Now, the other way you can approach your assembly level analysis is using manual contacts.
10:39
Now, with manual contacts, you have to go through,
10:43
and just like it says, you have to manually choose the primary and the secondary entity that are involved in the contact.
10:49
This gives you more insight and more control over the contact.
10:53
And the added benefit is you can group surfaces together.
10:57
So, where when you use automatic contacts, this generated like 14 or 15 contact sets.
11:03
With manual, you could probably get that down to probably three maybe four contact sets.
11:09
So, it will actually speed up the analysis time, but it does take more work on the front end.
11:16
So, ultimately, it will be worth the effort, but it's something that you'll want to get familiar with before using.
11:22
So, what I can do is I can start by choosing a primary entity.
11:26
And in this case, let's say I want to choose the pin as my primary entity.
11:32
I'll go ahead and select this pin face right here.
11:37
And what I can also do is choose the rest of the pin faces.
11:41
So, it's been split into a couple of faces.
11:43
I'm going to choose both of those.
11:45
And notice both of those are included in the primary entity box.
11:50
So, where automatic contacts only uses one surface at a time manual contacts allow you to choose multiple entities for that box,
11:58
and I can do the same thing with secondary entities.
12:01
So, where before it had a total of I think four or five contact sets just to define the interaction between the pin and the receiver and the hitch.
12:11
I can just go through and choose those faces.
12:19
And if it's choosing the wrong face, you can right click and do select "Other",
12:23
and allows you to choose the faces that are behind your cursor, which in this case, is this one here on the hitch.
12:29
Same thing on the other side.
12:31
I can right click, select "Other", choose the face that I want, which is that one right there.
12:39
And then lastly this one right here, which is going to be that face of the receiver.
12:44
So, I have two faces from the receiver, two faces from the hitch.
12:47
All of those can be your secondary entities.
12:49
And then these two faces here of the pin can be your primary.
12:53
And this will act as one contact set between those three components,
12:57
which is really going to simplify the number of sets you have in your analysis and keep things more clean and organized.
13:04
And it gives you a little bit more insight into what you're actually doing and how you're constraining and modeling the physics.
13:12
So, it's a very advantageous way to do this.
13:14
So, I'll select "Ok".
13:16
And now you'll notice surface contact 15 has been added.
13:18
I can also rename the contact, I could say Pin to Hitch Separation.
13:28
And that gives me a lot more information than just surface contact 15.
13:33
So, it gives you a little more control over that entire process.
Video transcript
00:08
In this demonstration, I will be covering contacts within Inventor Nastran,
00:12
as well as going through where they're best used and the settings involved with each type.
00:19
So, for this example, I'll be using this hitch assembly again here.
00:22
And taking a look at it, you can see that there are four individual parts or four individual bodies that have been modeled in the assembly.
00:29
So, if I go over to the model tree, you'll see those four-part files, you'll also see that relationships have been created.
00:37
So, these mates that have been added in within the assembly environment do not transfer to the FEA environment or Inventor Nastran.
00:46
So, I need to provide Inventor Nastran with information on how these individual parts interact with one another,
00:53
and what surfaces may come into contact or are welded or bolted together.
00:60
So, to do that with Inventor Nastran, I need to create what are called contacts or contact sets between each of those surfaces.
01:07
So, you'll see contacts is up on the ribbon here right next to setup and next to mesh settings.
01:13
If I do not activate any contacts and I select "Run", what you'll notice is it kicks off like a normal linear static analysis.
01:21
Everything looks Ok.
01:24
But then you'll get this E5000 series error.
01:27
So, if you ever get an E5000 or an E5004, double check that you have contacts applied and that these settings are correct.
01:36
If you do not have contact created, that means there's some level of instability or a singularity that's been detected.
01:42
So, what's really happening is this ball right here is getting pulled off into infinity,
01:47
the parts are separating and the solver is not able to calculate the stiffness of those interactions.
01:53
And so, it fails.
01:55
So, what we'll do is we'll add contacts to fix that problem.
02:01
So, I'll walk you through the two primary contact types, automatic and manual.
02:06
So, the way that automatic contact works is it uses a predetermined default tolerance range.
02:13
Any surfaces that fall within that range will be given a default contact type, which is typically bonded.
02:20
Now to find where that's at, you actually have to edit the analysis.
02:25
So, I'll right click and edit and then I'll go into the options tab right here and you'll see Contact data, Contact type is Bonded, Tolerance 0.0039.
02:37
This value is essentially 0.1 millimeters, but in inches, it's 0.00393.
02:44
And the contact type of bonded is what will be applied.
02:47
So, what this means is any surface of separate parts that are within 0.0039 will be assigned a bonded contact upon running auto contacts.
03:00
This works really well when you have a few parts that are relatively close to one another,
03:05
and you know, are going to be bonded, you can go back later and change them from bonded with separation.
03:11
This is a really good way to start because it'll make sure that things are held together.
03:15
And then you can work backwards, gradually releasing the degrees of freedom and allowing things to separate or slide as you go.
03:23
So, what I might do is leave the default contact tolerance as it is and just go ahead and run it to see what I get.
03:30
So, I'll select "Auto", it's going to detect contacts within that range.
03:36
And now there's a Surface Contacts folder that's been created in the analysis tree.
03:40
If I expand it, you'll see there's been 14 contacts created.
03:44
If you click on them, it'll show you the two faces that are in that set,
03:49
which in this case is the hitch to the receiver that has several faces on it.
03:54
Which means if I highlight that whole set of eight,
03:58
it's essentially the eight surfaces going around the outside of the hitch touching where it comes into the receiver.
04:07
The next set here is between the pin and the receiver, which is essentially going to be both sides where it passes through those holes.
04:16
I also have the hitch to the pin, pin to the receiver there on that side,
04:22
the chrome ball here where it is welded to the hitch and then the hitch to the pin on the other side.
04:28
So, what it's doing is it's going through and identifying all of those surfaces.
04:34
So, if you want to identify what this creates and what the result would be,
04:39
I recommend running it at least once to understand the effect of these bonded contacts on the stiffness,
04:46
and the ultimate result of this analysis.
04:48
So, I'll go ahead and select "Run" and this should eliminate that E5000 series error that I was getting.
04:55
I have a constraint, a load and now bonded contacts between all of the faces.
05:00
So, it should be a stable model.
05:04
So, I'll select "Ok".
05:06
And I should see this kind of bend downwards, create some stress on that filet there near the weld, about 10,000 psi of stress.
05:14
Everything up here is mostly rigid near the constraint.
05:17
And this pin and receiver is behaving very stiff.
05:22
And this is an area where maybe I consider switching from bonded to separation.
05:27
The issue with a bonded contact here is it's creating a welded connection where maybe I want to allow some level of sliding or opening.
05:35
So, we'll break down the contact types here and make a couple of changes in that region to potentially generate a better result.
05:43
So, I'll go ahead and unload these results and walk you through the different contact types before we make any changes.
05:49
So, if I go to manual contacts, you will see the contact type here.
05:55
There's a drop-down menu and there are a total of eight different contacts.
06:01
The most commonly used contacts are going to be your separation and your bonded.
06:04
Separation is going to allow the two surfaces to slide and rotate and separate from one another.
06:11
The only thing it does is it prevents surfaces from passing through one another.
06:17
So, just like if you were to put your pencil down on the desk in front of you, it can't pass through that surface.
06:23
That is a separation contact that has been generated.
06:26
Bonded contacts are essentially a weld that joins two surfaces together.
06:32
It connects the translational degrees of freedom of those nodes.
06:36
Sliding, no separation allows for sliding between parts, but they cannot separate intention or compression.
06:43
They can just slide in plain.
06:44
This is great for pinned connections.
06:47
Separation, no sliding can only be used in a nonlinear analysis.
06:51
And this is essentially infinite friction.
06:54
Offset bonded is great when you have two shell elements that have rotational degrees of freedom being bonded together.
07:01
So, shell to shell, shell to solid interactions or anywhere you have a fairly significant gap between surfaces.
07:10
Offset bonded is going to be a little bit more rigid and reliable than a traditional bonded contact.
07:16
But it's still considered a weld.
07:19
You also have shrink fit sliding and shrink fit no sliding.
07:21
These can only be used in nonlinear analysis when you have interference from a shrink fit.
07:27
And then you can also just disable the contact as well if you'd like to keep it in the list, but turn it off.
07:37
So, jumping back to the contacts in the list here,
07:42
I may change some of these to allow a little bit more realistic interaction between the parts where I have the pin coming through.
07:50
It's not being welded through the receiver.
07:53
The hitch is also not going to be welded to the receiver.
07:57
Those are free to slide, rotate and separate.
08:02
So, I want to change those to separation.
08:05
However, the hitch ball will be welded to the hitch at the end here.
08:11
So, that area I may leave as bonded because it will be welded in that region.
08:17
So, if I go ahead and I select all of these contacts here, I can go ahead and edit.
08:24
And notice when you do a group select, you can't change the entities that are involved or the name.
08:31
But what you can do is you can change the contact type here to separation and then select "Ok".
08:37
And you'll notice the icon changes from two blocks together to two that are offset and separated.
08:43
That is the icon you'd like to see there for separation.
08:47
So, that's been updated, I can then go through and update some of these other contacts as well if I'd like to.
08:52
But I'm going to leave, you know, potentially that chrome bone and hitch the same.
08:56
So, I might edit some of these other contacts here, make those separation as well.
09:04
So, that means a lot of things are able to separate and slide.
09:08
But ultimately, the weld here will keep this whole thing intact.
09:15
Now, when I solve this, because I'm allowing for more sliding and degrees of freedom, it will take longer to solve than a fully bonded model.
09:24
So, I'll select "Run" and then I'll come back and view the results when it's done.
09:30
So, after it solves, you'll see the result looks quite different.
09:33
I still have a very similar maximum stress in this area here near the hitch ball in the weld.
09:39
But notice, there's a little bit more bending sliding and then stress being applied here,
09:45
to where that pin is going to interact with the hitch receiver and the internal hitch there, which is what I would expect.
09:53
I'd expect there to be some pressure there where the load is transferred,
09:57
and some pressure here where it starts to bend before this whole area up here was blue because it was too rigid.
10:05
It was as though the entire surface was welded.
10:08
When in reality, those two surfaces can slide freely and the pin should be taking the majority of that sheer force due to the hitch ball.
10:18
So, I'm satisfied with that result, I can then go ahead and save my study.
10:22
And then from here you would continue on running a convergence analysis on the mesh and then you'd be ready to use that result for design purposes.
10:34
Now, the other way you can approach your assembly level analysis is using manual contacts.
10:39
Now, with manual contacts, you have to go through,
10:43
and just like it says, you have to manually choose the primary and the secondary entity that are involved in the contact.
10:49
This gives you more insight and more control over the contact.
10:53
And the added benefit is you can group surfaces together.
10:57
So, where when you use automatic contacts, this generated like 14 or 15 contact sets.
11:03
With manual, you could probably get that down to probably three maybe four contact sets.
11:09
So, it will actually speed up the analysis time, but it does take more work on the front end.
11:16
So, ultimately, it will be worth the effort, but it's something that you'll want to get familiar with before using.
11:22
So, what I can do is I can start by choosing a primary entity.
11:26
And in this case, let's say I want to choose the pin as my primary entity.
11:32
I'll go ahead and select this pin face right here.
11:37
And what I can also do is choose the rest of the pin faces.
11:41
So, it's been split into a couple of faces.
11:43
I'm going to choose both of those.
11:45
And notice both of those are included in the primary entity box.
11:50
So, where automatic contacts only uses one surface at a time manual contacts allow you to choose multiple entities for that box,
11:58
and I can do the same thing with secondary entities.
12:01
So, where before it had a total of I think four or five contact sets just to define the interaction between the pin and the receiver and the hitch.
12:11
I can just go through and choose those faces.
12:19
And if it's choosing the wrong face, you can right click and do select "Other",
12:23
and allows you to choose the faces that are behind your cursor, which in this case, is this one here on the hitch.
12:29
Same thing on the other side.
12:31
I can right click, select "Other", choose the face that I want, which is that one right there.
12:39
And then lastly this one right here, which is going to be that face of the receiver.
12:44
So, I have two faces from the receiver, two faces from the hitch.
12:47
All of those can be your secondary entities.
12:49
And then these two faces here of the pin can be your primary.
12:53
And this will act as one contact set between those three components,
12:57
which is really going to simplify the number of sets you have in your analysis and keep things more clean and organized.
13:04
And it gives you a little bit more insight into what you're actually doing and how you're constraining and modeling the physics.
13:12
So, it's a very advantageous way to do this.
13:14
So, I'll select "Ok".
13:16
And now you'll notice surface contact 15 has been added.
13:18
I can also rename the contact, I could say Pin to Hitch Separation.
13:28
And that gives me a lot more information than just surface contact 15.
13:33
So, it gives you a little more control over that entire process.
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in to start learning
Sign in for unlimited free access to all learning content.Save your progress
Take assessments
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement. May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.