Symmetry/Centering constraining

[Anonymous]

Hello,

My question regards constraints in the assembly environment.

The symmetry constraint of course exists and to my understanding of it, takes two components or geometry details and places them symmetrically about a plane. I want to do the opposite essentially, take one component and place it centered between two planes or faces.

I have not been able to find a single command like the symmetry constraint to accomplish this. Currently I have been measuring components and offsetting with a normal mate or flush to achieve centering the component between two faces. Does there not exist a constraint way to select my component, select the two faces and have the component placed in the middle?

Thanks for any insight!

(I've only been using Inventor for a couple months)

[Anonymous]

Hello,

My question regards constraints in the assembly environment.

The symmetry constraint of course exists and to my understanding of it, takes two components or geometry details and places them symmetrically about a plane. I want to do the opposite essentially, take one component and place it centered between two planes or faces.

I have not been able to find a single command like the symmetry constraint to accomplish this. Currently I have been measuring components and offsetting with a normal mate or flush to achieve centering the component between two faces. Does there not exist a constraint way to select my component, select the two faces and have the component placed in the middle?

Thanks for any insight!

(I've only been using Inventor for a couple months)

[blandb]

Symmetry constrain will not allow you to choose your first 2 selections on the same part. You can create a bisecting work plane between you other planes, so if one moves, the bisecting plane always remains centered and can constrain to this, or the same process between 2 faces, just create a bisecting plane of the 2 faces. If you parts a modeled around the origin, then you will have centered planes to use there as well.

[blandb]

Symmetry constrain will not allow you to choose your first 2 selections on the same part. You can create a bisecting work plane between you other planes, so if one moves, the bisecting plane always remains centered and can constrain to this, or the same process between 2 faces, just create a bisecting plane of the 2 faces. If you parts a modeled around the origin, then you will have centered planes to use there as well.

[jtylerbc]

The Symmetry constraint isn't usually described this way, but can achieve what you want in at least some cases.

• The two green plates were placed first, and constrained to each other.
• I then added the red plate, intended to be centered between the green ones. 
• Since the green ones were already constrained, when I added the Symmetry constraint, it was the red plate that moved (essentially solving the Symmetry constraint backwards to how it is normally used).

I believe that doing it this way can be a little finicky depending on what other constraints are on the parts (at least it was in earlier versions - this issue may have cleared up since then).  It may not solve all of your cases, but may handle some of the simpler ones.

If you can post some screenshots of a real application where you need to do this, you might get more suggestions for ways you could handle it. 

[jtylerbc]

The Symmetry constraint isn't usually described this way, but can achieve what you want in at least some cases.

• The two green plates were placed first, and constrained to each other.
• I then added the red plate, intended to be centered between the green ones. 
• Since the green ones were already constrained, when I added the Symmetry constraint, it was the red plate that moved (essentially solving the Symmetry constraint backwards to how it is normally used).

I believe that doing it this way can be a little finicky depending on what other constraints are on the parts (at least it was in earlier versions - this issue may have cleared up since then).  It may not solve all of your cases, but may handle some of the simpler ones.

If you can post some screenshots of a real application where you need to do this, you might get more suggestions for ways you could handle it. 

[Anonymous]

Thanks for the helpful insight!

I will try to explain the application and convenience I am looking for better.

I am looking for quick ways to place components in assemblies "in the middle" of various geometry. Sometimes the planes I want to center a component about are on the same part and sometimes not. I am trying to avoid measuring and offsetting from one end, even though it is simple to do so, I am looking for something faster and more convenient/efficient. Creating new planes in the middle of the component is certainly a useful idea and thank you for that. Here are a couple examples that illustrate fairly well the types of situations I have.

The example here would be to center the colored component pattern about the faces of the channel flanges. Instead of offsetting a specified distance from one of the flange faces to place the component in the center I am looking for commands to just place it in the center without needing to specify distances. Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint). For example I do not understand why I cannot use the midplane command and select both flange faces of the channel. It is still not very efficient to create a midplane by offsetting from one side of the part as a solution to having to offset the part to center it in the first place.

The difference is this example is that I am trying to center about faces on different parts unlike the previous. The dark colored pipes is the component pattern in which I am centering between the angle iron on the outsides (or centering between the channels, same thing). Here I can also not create midplanes on either the component pattern or components of the frame (the frame is the channel and angle etc). The frame is one component within my assembly so I suppose that is why I cannot create a midplane between the two channel, just as I could not on an individual channel?

Again of course it is simple enough to measure and offset to reach the goal of a centered component but I am hoping there are better ways. Thank you for the input so far, it is appreciated.

[Anonymous]

Thanks for the helpful insight!

I will try to explain the application and convenience I am looking for better.

I am looking for quick ways to place components in assemblies "in the middle" of various geometry. Sometimes the planes I want to center a component about are on the same part and sometimes not. I am trying to avoid measuring and offsetting from one end, even though it is simple to do so, I am looking for something faster and more convenient/efficient. Creating new planes in the middle of the component is certainly a useful idea and thank you for that. Here are a couple examples that illustrate fairly well the types of situations I have.

The example here would be to center the colored component pattern about the faces of the channel flanges. Instead of offsetting a specified distance from one of the flange faces to place the component in the center I am looking for commands to just place it in the center without needing to specify distances. Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint). For example I do not understand why I cannot use the midplane command and select both flange faces of the channel. It is still not very efficient to create a midplane by offsetting from one side of the part as a solution to having to offset the part to center it in the first place.

The difference is this example is that I am trying to center about faces on different parts unlike the previous. The dark colored pipes is the component pattern in which I am centering between the angle iron on the outsides (or centering between the channels, same thing). Here I can also not create midplanes on either the component pattern or components of the frame (the frame is the channel and angle etc). The frame is one component within my assembly so I suppose that is why I cannot create a midplane between the two channel, just as I could not on an individual channel?

Again of course it is simple enough to measure and offset to reach the goal of a centered component but I am hoping there are better ways. Thank you for the input so far, it is appreciated.

[blandb]

Model everything about and origin. That way you will always have planes and axis running through the center of your parts, then you can use these origin planes to constrain components together. Sometimes will have to constrain from one end by a certain amount, you cant always avoid that, but as for centering you have origin planes. Just like your example of the black pipes, you can use the origin planes of the plate and the origin planes of the black tubes, constrain them together, and use the faces to place the black tube where it belongs. Component pattern using mid option. But if it in not symmetrical in both ways, you may have to change the first instance location and use the edge of the plate, all depends on geometry and what you are trying to achieve.

[blandb]

Model everything about and origin. That way you will always have planes and axis running through the center of your parts, then you can use these origin planes to constrain components together. Sometimes will have to constrain from one end by a certain amount, you cant always avoid that, but as for centering you have origin planes. Just like your example of the black pipes, you can use the origin planes of the plate and the origin planes of the black tubes, constrain them together, and use the faces to place the black tube where it belongs. Component pattern using mid option. But if it in not symmetrical in both ways, you may have to change the first instance location and use the edge of the plate, all depends on geometry and what you are trying to achieve.

[jtylerbc · Accepted solution]

What @blandb said is correct, and I'll expand a little on what he said.

---

@Anonymous wrote:

Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint).

If that is a Content Center channel, you don't need to create a plane at all.  Just use the origin plane that is already there.  If it is a channel you modeled yourself, it should have been modeled around the origin, and then you'd be able to do the same thing.  So there is almost certainly no reason to create a new plane for the channel case, assuming the models were created in a reasonable way.

The one and only exception would be if some of the parts are imported geometry, and came in with their coordinate systems in goofy places as a result of the file translation.  Then you would need to create your own midplane, which brings us to addressing the following:

---

@Anonymous wrote:

Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint).

---

That is only true if you try to create that plane at the assembly level.  If you use the same midplane command in the part itself, it will work just fine.  Again, unless this is imported or badly modeled geometry, you probably don't need to.  But if necessary, it is possible at the part level.

---

@Anonymous wrote:

For example I do not understand why I cannot use the midplane command and select both flange faces of the channel.

As I mentioned, you can do this if you do so at the part level instead of the assembly.  The reason you can't do it at the assembly level is actually very simple.  The current Symmetry constraint does not allow you to pick faces from the same part for Selection 1 and Selection 2.  When you use the Midplane command at the assembly level, the plane is positioned using an automatically-created Symmetry constraint, so it is limited by the rules that apply to that constraint.

In summary:

• Model parts around the origin whenever possible, so the origin planes will be in reasonable locations for constraining parts.
• Use the origin planes for constraining if they are in a reasonable location, rather than making new planes.
• If you do need to make new planes for some reason, do so at the part level, not at the assembly level. 
• The assembly won't let you create planes between faces on the same part, but the part is a more logical location for the plane to reside anyway.  Think about it like this:  Even if the assembly did let you create the midplane on the channel, it would exist only on that one instance of the channel.  All other copies of the channel would still be missing the midplane.  If you create that plane in the channel part itself, then all instances will have it, no matter how many copies of the channel are in the assembly.

[jtylerbc · Accepted solution]

What @blandb said is correct, and I'll expand a little on what he said.

---

@Anonymous wrote:

Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint).

If that is a Content Center channel, you don't need to create a plane at all.  Just use the origin plane that is already there.  If it is a channel you modeled yourself, it should have been modeled around the origin, and then you'd be able to do the same thing.  So there is almost certainly no reason to create a new plane for the channel case, assuming the models were created in a reasonable way.

The one and only exception would be if some of the parts are imported geometry, and came in with their coordinate systems in goofy places as a result of the file translation.  Then you would need to create your own midplane, which brings us to addressing the following:

---

@Anonymous wrote:

Creating a plane to accomplish this certainly works in the ways your replies have described but I find I run into a similar problem as Inventor does not allow, using the create midplane command, to select two faces on the same part(and of course almost the exact same problem with the symmetry constraint).

---

That is only true if you try to create that plane at the assembly level.  If you use the same midplane command in the part itself, it will work just fine.  Again, unless this is imported or badly modeled geometry, you probably don't need to.  But if necessary, it is possible at the part level.

---

@Anonymous wrote:

For example I do not understand why I cannot use the midplane command and select both flange faces of the channel.

As I mentioned, you can do this if you do so at the part level instead of the assembly.  The reason you can't do it at the assembly level is actually very simple.  The current Symmetry constraint does not allow you to pick faces from the same part for Selection 1 and Selection 2.  When you use the Midplane command at the assembly level, the plane is positioned using an automatically-created Symmetry constraint, so it is limited by the rules that apply to that constraint.

In summary:

• Model parts around the origin whenever possible, so the origin planes will be in reasonable locations for constraining parts.
• Use the origin planes for constraining if they are in a reasonable location, rather than making new planes.
• If you do need to make new planes for some reason, do so at the part level, not at the assembly level. 
• The assembly won't let you create planes between faces on the same part, but the part is a more logical location for the plane to reside anyway.  Think about it like this:  Even if the assembly did let you create the midplane on the channel, it would exist only on that one instance of the channel.  All other copies of the channel would still be missing the midplane.  If you create that plane in the channel part itself, then all instances will have it, no matter how many copies of the channel are in the assembly.

[Anonymous]

Thank you both so much! I definitely have a bit better understanding of the program now. Using the origin planes for constraining is absolutely the key thing I was never considering until now!

[Anonymous]

Thank you both so much! I definitely have a bit better understanding of the program now. Using the origin planes for constraining is absolutely the key thing I was never considering until now!

[ribo44]

Hey,

Sure it's easier said then done to model everything around the Center. Often parts are just not symetric to be modeled around the Center that is later used in the Assembly. And often I have to Center many different assemblys to each other, sometimes where the midplane is available on only one part of the Assembly.  Going into all single parts to create some planes and Show them in the Assembly to later hide them is realy time consuming. The Assembly i'm currently working took me around 25 minutes just to create Center planes. when we worked with NX it took me around two minutes to accomplish the same Thing. I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

[ribo44]

Hey,

Sure it's easier said then done to model everything around the Center. Often parts are just not symetric to be modeled around the Center that is later used in the Assembly. And often I have to Center many different assemblys to each other, sometimes where the midplane is available on only one part of the Assembly.  Going into all single parts to create some planes and Show them in the Assembly to later hide them is realy time consuming. The Assembly i'm currently working took me around 25 minutes just to create Center planes. when we worked with NX it took me around two minutes to accomplish the same Thing. I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

[jtylerbc]

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@ribo44 wrote:

I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

---

It's not very useful to make this complaint without explaining what "Basic feature" you're talking about.  You did not mention one at all - just that you could do it faster in NX, without any mention of what makes that possible.

Even if the part is not symmetric, modeling with some key feature (a mounting hole pattern, a drive shaft, etc.) located at the origin is generally a good practice. 

[jtylerbc]

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@ribo44 wrote:

I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

---

It's not very useful to make this complaint without explaining what "Basic feature" you're talking about.  You did not mention one at all - just that you could do it faster in NX, without any mention of what makes that possible.

Even if the part is not symmetric, modeling with some key feature (a mounting hole pattern, a drive shaft, etc.) located at the origin is generally a good practice. 

[ribo44]

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@jtylerbc wrote:

---

@ribo44 wrote:

I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

---

It's not very useful to make this complaint without explaining what "Basic feature" you're talking about.  You did not mention one at all

---

I was talking about the feature to use a "Center constraint" as stated in the original post.

And sure the best way is to model at the Center with the key features. But if the part is 4 or 5 assemblies down the line, to get there to Show/use the origin planes just takes up so much time.

[ribo44]

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@jtylerbc wrote:

---

@ribo44 wrote:

I'm very sad that the did not integrate such a Basic feature into Inventor 2020...

---

It's not very useful to make this complaint without explaining what "Basic feature" you're talking about.  You did not mention one at all

---

I was talking about the feature to use a "Center constraint" as stated in the original post.

And sure the best way is to model at the Center with the key features. But if the part is 4 or 5 assemblies down the line, to get there to Show/use the origin planes just takes up so much time.

[blandb]

You can use a part priority selection filter to select the part. Then use find in browser and turn on the origin. Repeat to turn off. Doesn't matter how deep the part is.

[blandb]

You can use a part priority selection filter to select the part. Then use find in browser and turn on the origin. Repeat to turn off. Doesn't matter how deep the part is.

[jtylerbc]

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@ribo44 wrote:
I was talking about the feature to use a "Center constraint" as stated in the original post.

---

Ah, okay.  I read your post as saying that the process of creating the center planes was faster in NX, without explaining why that was the case.  It seems that what you really meant was that you can skip that process altogether because of the "Center constraint" that's available there.

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@ribo44 wrote:
And sure the best way is to model at the Center with the key features. But if the part is 4 or 5 assemblies down the line, to get there to Show/use the origin planes just takes up so much time.

---

In addition to @blandb 's tips on faster ways to drill down to the part, there is often no need to turn the origin plane visibility on and off in the first place.  This is really only needed if you're going to constrain to it over and over.  For one-off constraints, you can just click the plane in the browser without ever changing the visibility state.

[jtylerbc]

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@ribo44 wrote:
I was talking about the feature to use a "Center constraint" as stated in the original post.

---

Ah, okay.  I read your post as saying that the process of creating the center planes was faster in NX, without explaining why that was the case.  It seems that what you really meant was that you can skip that process altogether because of the "Center constraint" that's available there.

---

@ribo44 wrote:
And sure the best way is to model at the Center with the key features. But if the part is 4 or 5 assemblies down the line, to get there to Show/use the origin planes just takes up so much time.

---

In addition to @blandb 's tips on faster ways to drill down to the part, there is often no need to turn the origin plane visibility on and off in the first place.  This is really only needed if you're going to constrain to it over and over.  For one-off constraints, you can just click the plane in the browser without ever changing the visibility state.

[ribo44]

In addition to @blandb 's tips on faster ways to drill down to the part, there is often no need to turn the origin plane visibility on and off in the first place.  This is really only needed if you're going to constrain to it over and over.  For one-off constraints, you can just click the plane in the browser without ever changing the visibility state.

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That might actualy help. It is still not the ideal solution for me. But my hopes are high that it might come eventualy in the future.

[ribo44]

In addition to @blandb 's tips on faster ways to drill down to the part, there is often no need to turn the origin plane visibility on and off in the first place.  This is really only needed if you're going to constrain to it over and over.  For one-off constraints, you can just click the plane in the browser without ever changing the visibility state.

---

That might actualy help. It is still not the ideal solution for me. But my hopes are high that it might come eventualy in the future.