Moving holes in an assembly?

Is this possible? One of our mentors wants us to make the control board in autodesk. He says in AutoCAD he can make the drill pattern and drill through everything, including other parts. He wants us to make it in Inventor, but none of us know how.

Help would be appreciated.

If you know where the holes go in part A, and where part B is in relation to part A, you should have no problems putting the holes where they belong in part B.

As for putting the holes straight through everything without individually modifying each part, as far as I know, you can’t do that.

It’s been awhile since I’ve used Inventor, but there are two things you should be able to do to achieve the desired result.

You can create and define the hole pattern you’d like in one of the parts and simply create, but do not define, them in a second. That means, essentially, that one part is fully dimension and fixed while the second has holes in it, but no dimensions placing them in a certain location. In the second part, set the hole feature as adaptive and, at the assembly level, the holes should move to match the defined holes in the first part when they’re constrained together.

You also may be able to create an assembly of the two parts and, at the assembly level, create a new sketch and feature for the holes.

The former is probably the better method, but as I said, it’s been awhile since I’ve used it and the exact process may be somewhat different.

in assembly, you can put a new 2D sketch on the top part where the hole goes, and then tell the hole to go THROUGH ALL, and it will. there should be a hole of the same diameter thtough both (or all) parts in the line of fire of the hole that are in that $@#$@#$@#'y.

I have another way to do this and i just checked it out and it work so here goes.

In your top level assembly create a work plane on the top part that you want to put holes in. Now you can create a new sketch on that work plane, dimension it to the visible geometry of the part and then extrude “through all.” what this will do is it will put a hole in every part beneath the work plane and then when you save the parts out the hole will be saved as projected geometry. This is good because it will take that hole and individually apply it to each sub part without you having to go though and do it individually.

Hope this helps.

I’ve played around with the two best methods for doing this:

Greg’s method will work. I haven’t been able to duplicate exactly his results though. Using V10, features placed in a top level assembly do not reflect as features in the affected parts. Therefore, as I follow Greg’s procedure, the original .ipt files would not be modeled with the holes present, although they would appear in the assembly. It still works, and it’s easy to understand and implement, but it can cause problems later on. This method lets you produce an assembly that has the features present with out modifying the original parts. This can be helpful and it can be detrimental. It is helpful if you are unsure of where to place the holes, if you have similar parts that might be used again in another assembly and you don’t want multiple copies of slightly different parts, or multiple proposed versions of the hole pattern (as in multiple assembly’s with the same parts and different hole patterns in each assembly). It’s a nice way to quickly play with features with out worrying about keeping parts ‘jiving’ with one another. However, when you do decide on a hole pattern, and you start marking up your part drawings (.dwg’s), you’ll find that the holes are not present in the original parts. This may or may not be a problem for your purposes, since you might not even be using printed drawings of the parts, but it would get me a serious ear full from my CAD instructor if I turned in a project with high level assembly features like that in place of fully featured parts.

I would probably use M.Krass’s method, as it is the most adaptive to future changes. By driving one feature with another features constraints, you can make quick changes to the feature, or eliminate that adaptivity if you no longer want them to line up and have it all reflected in the original .ipt’s. The end result are fully modeled parts that look just like they should when finished. It uses the best technique, and there is much to be said about that. Still, it requires some skill to properly apply all the constraint, time to modify each part and the abstract thinking to keep it all straight in your head.

So, it comes down to how much effort you want to put into this. One method is quick and ‘dirty’ (not to disparage the method) the other is slower and ‘cleaner’. My guess is that since this is ‘just’ an OI piece, the extra work required to make an easier to understand part drawing and more adaptive part file probably isn’t worth it, and Greg’s method is a better pick. He may have a setting in effect that would save assembly features into individual parts, although I can’t figure it out. Perhaps an earlier version of Inventor?

Any hints Greg?

-Andy A.

What I would do is create and constrain an assembly - for instance: Part1 and Part2. Edit Part1 to include your holes. Edit Part2 and create a sketch. Use the Project Geometry tool to project the hole geometry from Part1 to the sketch on Part2. Finish the sketch and extrude the holes on Part2. Save Part2. You can now change the sketch for your holes on Part1 and the holes on Part2 will follow and be savable for your drawings.

I think this is similar to M. Krass’ solution. Maybe explained a bit differently.

One method I found to be very effective, is to use the Design Accelerator feature of Inventor 10.

While in the assembly, there is a button with a picture of a blue bolt on the side panel. If you click on it, it will take you to a new window where it asks you to define nuts, bolts, washers etc.

I assume you will want to put bolts through the holes, so it should make it alot easier. But if you just want the holes, I’m pretty sure that you can only select to create holes without anything else. But if you can’t, you could always create it with the bolt, and on the Browser Panel, delete the bolt. That will keep the holes there.

I think this could clear up what Eric was asking

We will be putting holes through a control board. We want each of are parts on the control board to have a bolt pattern and wire patter. This is how we could easily find if there’s space for the holes of diffrent parts. example; partA has 5 hole around it that pass through the control board, where wires will go through, we want to be able to see how much room we have to add a partB with its own holes. Also, using this could save time, if partA is used 5 times we don’t want to have to repeat the hole cut over and over.
How could this be Done?

If the holes were applyed on a 2D sketch with in the Part, then in the assembly could we apply the extrusion through the board? How?

"If the holes were applyed on a 2D sketch with in the Part, then in the assembly could we apply the extrusion through the board?

Yes and no.

“How?”

You would not “apply the extrusion through the board.” In your assembly you should have the board mated to the Part. Within the assembly, start a new sketch on the board. Use the Project Geometry tool to project the holes from the Part on to the sketch. Extrude the holes through the board. The holes on the board will now be adaptive to the holes in the Part.

Does this not solve your problem or am I missing something here.

Thanks alot everyone! W solved the problem thanks to your posts!