Updating constraints based on other dimensions in an assembly

[meke42]

I'm pretty new to Inventor so I please apologize if the answer to my question could be found somewhere. I have the problem that in many of my assemblies I have to update a lot of constraints and dimensions if I change the size of single elements and I have the feeling that there is better ways of doing this than what I do now (i.e. manually update all the relations).

Example 1) Imagine a rectangular baseplate with dimensions 800 mm x 200 m. I want to equally distribute 4 components over the plate with 200 mm distance. From the edge of the plate to the first/last component I want to maintain a distance of 100 mm, i.e. the total construct adds up to exactly the 800 mm of the plate. See figure below.

So far I'm usually using a rectangular pattern to do this, where I have to manually enter the distance between the components (200 mm). The initial component I then constraint with a flush/mate constraint to the edge of the plate. This works fine, however, the problem starts if I change the dimensions of the plate, e.g. expanding the plate to 1000 mm instead of 800 mm. I now have to manually adapt the spacing between the components and do this every time I update the plate size.

Is there a way to automate this, i.e. to tell Inventor to change the spacing based on the dimensions of the plate such that it always equally distributes the components over the entire space which is given by the dimension of the plate?

A similar problem also arises if I want to center constraint two objects (example 2):

I want the gray and the ocher colored objects to share the same centerline. For that I use a flush constraint as illustrated on the right figure, where I have to manually calculate the width difference. As soon as one of the two dimensions changes, I have to manually change the flush constraint again. I tried to introduce a workplane ("midplane between two planes") for each object, but for some reason (why?) inventor doesn't allow me to select two faces of the same part to construct a centerplane for this part (is there a way to do this?). What would be a better way of doing this?

[swalton · Accepted solution]

A few questions..

1.  Are you modeling the grey and brown parts symmetric about their origin geometry?
   1. If so, use a flush or mate constraint between the proper origin workplanes on the two parts.
   2. If not, why not?
2. Patten of components on the big plate:
   1. Create a feature pattern in the big plate to locate the other component in your assembly. 
   2. I usually use a mounting hole, or tab-and-slot, or even just a work plane and the base feature
   3. Use the parameters window to create the proper equations to locate the base feature and patterned members.
   4. Adjust the big plate size a few times to confirm that the pattern adjusts as expected.
   5. In the assembly, constrain the 1st instance of the other part to the seed feature of the pattern.
   6. Use a feature -driven pattern in the assembly to add the rest of the parts.
   7. Any time you adjust the overall length of the big plate, the location and number of the other part will follow the changes in the feature pattern.

[jtylerbc · Accepted solution]

I'm going to answer your second issue first, as I recently had a user in my office making the same mistake so it's fresh on my mind.  If I have time later, I'll come back give some pointers on the first scenario.

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@meke42 wrote:

A similar problem also arises if I want to center constraint two objects (example 2):

I want the gray and the ocher colored objects to share the same centerline. For that I use a flush constraint as illustrated on the right figure, where I have to manually calculate the width difference. As soon as one of the two dimensions changes, I have to manually change the flush constraint again. I tried to introduce a workplane ("midplane between two planes") for each object, but for some reason (why?) inventor doesn't allow me to select two faces of the same part to construct a centerplane for this part (is there a way to do this?). What would be a better way of doing this?

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Inventor doesn't let you create the plane you are describing from within an assembly.  That is because assembly work planes are created using constraints, so by selecting the same part twice, you are essentially telling Inventor to constrain a part to itself.

What you should be doing is creating that plane in the part, not the assembly.  This will also allow that plane to exist in all future assemblies where that part is used, rather than only existing in the assembly where you created it.  It really only makes sense to create a plane at the assembly level if it is between different parts.

Further, what would really be preferable is that you build the part symmetric about the origin to begin with.  This would allow you to constrain the part the same way you are describing, but using an origin plane that already exists instead of needing to create a work plane.

[johnsonshiue]

Hi! I guess OP wants to work around the lack of SWX' Width Mate in Inventor. I think the best workaround is creating mid plane in those parts. Simply mate or flush the mid planes.

Another way is to leverage iLogic rule to drive parameters at different levels.

Many thanks!

[meke42]

Thanks for the hint on drawing the component symmetrically around its origin, which would actually have been a very straight forward idea I probably should have realized by myself.

Unfortunately I can't really follow the answer for 2). What should I use the feature pattern in the plate for? And why do I need an additional feature pattern in the assembly? I don't really understand what you mean by "use a mounting hole, or tab-and-slot, or even just a work plane and the base feature"? Can you maybe explain what the basic idea of this solution would be such that I can try out to do what you wrote until I figure it out the details?

[swalton]

In your OP, you said that you wanted to components in the assembly to move automatically when you changed the size of the base plate.

The assembly file does not know anything about the size of the base plate.  There is a dimension/parameter in the base plate that defines the overall length.  By building a feature pattern in the base plate, you can write some parametric equations that define how the pattern changes as the overall length changes.  If you need to keep a 200mm spacing between assembly components, you can write an equation for the number and spacing of the feature pattern that keeps the instances 200mm apart and varies the 100mm dimension as necessary.

Once the equations work correctly, you can place the base plate at the origin of an assembly.  Then add a single instance of the component that is spaced on the base plate.  Constrain that component to the original feature of the base plate pattern, then create a Feature-Driven pattern using the component and the feature pattern.  Inventor will place an instance of the component at every instance of the feature in the pattern.  

Later, if the base plate changes from 800mm to 1000mm, the feature pattern will automatically adjust following the equation, and the components in the assembly will automatically follow the feature pattern.

I recommend making the feature in the base plate something that you need anyway.  Think a mounting hole, or a locating tab or similar.  The folks building the assembly need those features, so using them in the feature pattern reduces the work you have to do to create the model.

See the attached Inventor 2022 part for an example.