Line up of holes, shared/reused geometry in parts. I feature?

[mailswamp]

Hello.

I am designing a specialized tool. It would be a spreader for taking apart a connector.

I have two points on one part.

I would like to have the same two points projected on another part in the assembly.

I would like two parts to have holes that line up and I would like to build the second part around those two points.

Is it done through I feature? What tab of the I-feature menu do I tinker with to share two points across several parts in the assembly.?

Also I remember that there is a way to cut a hole through several parts. How do I do that?

I may not want to use that.

Those points would have shoulder bolts or pins or rivets running through them. (I will have to talk to the manufacturer.)

I watched the whole TEDCF videos course last year and I already forgot everything. I cannot even find how to do it using their search tool.

I forgot the term for it.

THANK YOU!!!

[johnsonshiue]

Hi! If I understood your requirement correctly, iFeature should not be relevant here. iFeature is basically a collection of features recipe stored in a file. Then it can be inserted to different parts without having to recreate the features.

What you are looking for is cross-part associativity. In Inventor, there are two main workflows to achieve that: Adaptive and Derive (Multi-Solid Body).

For Adaptive, you can project geometry from one part to another part. Or, you can create an adaptive sketch and use assembly constraint to align the sketch on one part to geometry on another part.

For Derive (Multi-Solid Body), you will essentially design the assembly in a part. Each body represent a geometrically unique part. Likewise, you can use sketch to represent a part or a subassembly. Then you derive the body or the sketch as individual part.

There is a a lot of good information about Adaptive and Derive on Autodesk Knowledge Network. Please take a look and try it out. Let us know if you have specific questions.

Many thanks!

[mailswamp]

I try to derive the part (pink lines) that goes over blue and green cylindrical extrusions (two variations of the same I part).

Then I get a message that tells me that I cannot do this.

I made those cylindrical extrusions "adaptive" and that did not change anything.

I cannot select cylindrical surfaces and surrounding geometry and offset a surface.

How do I do that? I may need to do this operation on more complicated parts (i.e. ball joints, 3D printable threads, etc)

Thank you.

[johnsonshiue]

Hi! Could you attach the files here or send them to me directly ([email protected])? I would like to understand why it does not work.

Many thanks!

[mailswamp]

I am trying to have Long Arm Top.ipt fit all surfaces of Pencil center.iam with a small gap in between.

There may be a simpler way to do this, however I would like to know how to use surface of two parts, make an offset and build a third part around that offset.

Thank you

[johnsonshiue · Accepted solution]

Hi I think I know what you want now. You want the cylindrical faces in Pencil Clamp to drive the hole diameter in the Long Arm TOP. If yes, this can be done is a few ways. The quickest way is probably Adaptive. Here is what you need to do.

1) Edit Long Arm Top.ipt and edit the sketch. It should be fully constrained.

2) Show All Constraints. Remove the equal constraint to the circle diameter. Finish edit. This will free up the needed degree of freedom.

3) Right-click on the extrusion -> check Adaptive.

4) Go back to the assembly.

5) Mate Constraint -> pick the cylindrical face (not the axis) in the Pencil Clamp-01 and pick the hole face in the Long Arm TOP.

Now when the diameter of the cylindrical face in the Pencil Clamp-01 changes, the hole in the Long Arm TOP will follow.

Another way is to use iLogic. At the assembly level, create an iLogic rule. Write the following code.

Parameter("Long Arm TOP:1", "d6") = Parameter("Pencil Clamp 01-01:1", "d8")
iLogicVb.UpdateWhenDone = True

Save and Run. The hole diameter in the Long Arm TOP will follow the cylinder in the Pencil Clamp-01.

There are other similar ways like derive or link the parameters from Pencil Clamp-01 to Long Arm TOP. But, Pecil Clamp is an iPart, which can make it a bit complicated.

Many thanks!

[mailswamp]

Thank you very much.

I would still like to know how to imprint a face of the assembly onto a part that I would like to add to the assembly.

Not all shapes are as simple as those cylinders in this example.

[johnsonshiue]

Hi! You could use Copy Object command to associatively copy geometry from Part A to Part B in an assembly (go to Modify tab -> expand the panel -> Copy Object). It should work just like adaptive feature but it is more at the face or body level.

Many thanks!

[mailswamp]

What is mate constraint?

Is it found under the regular assembly constraint?

I want 0.08mm gap for parts to move freely. How do I add that into this relationship?

[johnsonshiue]

Hi! Yes, Mate is the default constraint type in Assembly Constraint dialog. To have some allowance, you can expand the dialog and set Min and Max to the given constraint.

Many thanks!

[mailswamp]

I did what you told me and nothing happened. I cannot get the mate constraint to change the hole diameter in adaptable sketch.

[johnsonshiue]

Hi! I took a look at the latest iteration, I don't think it will work. You are trying to make adapive iPart. Long Arm TOP has been converted to an iPart factory. Then you want to make one of the feature adaptive within the iPart. iPart is for generating library content. Its definition has to be specified on the table. There should not be any driving force to change the shape from outside.

I am sorry I am little bit lost on what you are trying to do now. Could you explain to me why Long Arm TOP has to converted to an iPart factory?

Many thanks!

[mailswamp]

The part of Inventor that is in charge of relationships of parts is counter-intuitive.

I wish that I could communicate my vision on how to make it very easy to follow to the developer team.

We live in the world where every capitalist thinks that they know better. than others.

A "conform" command should be added to the software.

I am trying to make holes in the linkage arm follow the diameter of the cylindrical surface on either sides of the clamp.

(All holes will be defined by cylindrical surface diameter since all holes in link arms are set to be equal.)

I have a problem achieving this result.

This whole project is an exercise on how to relate parts to one another.

[johnsonshiue]

Hi! I did offer a few workflows to do what you are looking for. But, when you started converting the parts to iParts, some limitations will come. iParts are supposed to be more like library parts. The dimensions should be clearly defined on the author table. They should not be driven by something else. Could you tell me why you want to make them iParts?

Regarding knowing more than others, I personally do not claim that I know our customer workflows better. But, I know how Inventor works well and what it cannot do. I am trying to show you the ways this can be done in Inventor avoid further confusion. Certainly, Inventor always has room for improvement and there will always be limitations. The most important thing is to find the reliable workflows leading to desirable result.

Many thanks!

[mailswamp]

I-parts cannot have adaptive hole diameters?

[johnsonshiue]

Hi! No, unfortunately, iPart is more like library part. The geometry has to be clearly defined on the iPart table. Its definition has to be driven by iPart factory. I assume that you would like to have iPart member hole matched the cylinder. You will need to clearly specify the diameter for each member on the table. Then make sure the right member clamp matches the right member arm.

Many thanks!

[mailswamp]

I would like to create an indentation in the "nest" part for the "mother" and "father" part in the assembly. How do I accomplish this?

I would like there to be an adjustable gap between "mother" and "father" part and the "nest" part.

How do I achieve this?