I'm uncertain on how to proceed here, at least efficiently.
Here's the scenario:
I have a variety of objects of different sizes going into a foam filled case. The foam consists of several layers. In this instance there are 7 layers, 2 inches thick or thereabouts. I have the objects arranged in a way that the fit in the smallest footprint possible, and so that they are balanced inside the case.
Each object has a sketch drawn, at the part level, of the 'footprint' of the object. This is the cutout that will get cut into each layer of the foam, creating a hollow cavity for the object to sit in.
My conundrum though, is how to do this in the most efficient way possible. as this is something we do here at my company on a regular basis.
In Solidworks (cue eye-rolling), I would have simply picked each of the sketch profiles here in the assembly level, extruded each cavity down through the layers at the varying depths which they require, and choose whether or not I want the feature to show up at the part level. At this point I'd be done with this operation, and on to producing the 2D drawing and exporting die files for the mill to cut. This is not possible in Inventor.
Currently, I have to create another sketch here in the assembly level using Project Geometry to select the profiles I need to extrude. I have to do this over and over for each of the different depths I have to extrude. It would be handy if sketches were shareable in assemblies, not sure why it isn't. In this instance, I'd have to create 3 new sketches for each of the three different depths. God help me if I have to revise the outline, because it might not cascade correctly to the new sketches I have to create. After the additional sketches are created, I can extrude through the layers of foam. As you all know, it won't show up at the part level of the foam, so I have to use the Feature Migrator in the app store to push those extruded features to the individual layers. If a change is required to the outline at this point, it is a huge hassle. I'd have to go to each individual foam layer part and delete the migrated feature, then in my assembly, unsuppress the original extrusion feature, delete it (taking care not to delete the sketches along with it) and do the process all over again. As you can see, frustration can run really high.
So my prognosis is, either Inventor is sorely lacking in some of it's "parametric" abilities, or I am missing some sort of work flow that would make this process so much easier. I have posted a pic of the assembly below so that you all can get a better idea of what I'm talking about. Post up with your answers and suggestions!
Solved! Go to Solution.
Solved by cwhetten. Go to Solution.
Derived Component might be your easiest technique
or
Edit part in context of assembly, Copy Object - surface and Sculpt
or
Mutlibody solids master modeling techniques and push out the assembly.
I think there is an add-in somewhere to push assembly level features to part level, but as that is not correct technique in my opinion, I have never tried it out. Edit: Upon closer read - I see you have found the add-in.
Post your assembly here if you can't figure out technique 1, 2 or 3.
Hi RDG3PO,
This video might give some ideas:
http://www.youtube.com/watch?v=6JpK2bEJP-I&list=PL35F652F420934D61&feature=share
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
@Curtis_Waguespack wrote:Hi RDG3PO,
This video might give some ideas:
http://www.youtube.com/watch?v=6JpK2bEJP-I&list=PL35F652F420934D61&feature=share
Hey Curtis, thanks for posting the link. I'm familiar with it, and it has helped, to a degree. But our facility doesn't 3D mill the foam, its cut out from a profile, and the layers of foam are stacked to provide depth. If we ever upgrade to a 3D milling operation, this is the method we'd probably use, except it requires that the foam layer and the object be in the same part file, which means, doing a lot of copy/subtract bodies operations, considering we've put as many as 30 objects in a billet of foam that's comprised of 7 layers.
@Anonymous wrote:Derived Component might be your easiest technique
or
Edit part in context of assembly, Copy Object - surface and Sculpt
or
Mutlibody solids master modeling techniques and push out the assembly.
I think there is an add-in somewhere to push assembly level features to part level, but as that is not correct technique in my opinion, I have never tried it out. Edit: Upon closer read - I see you have found the add-in.
I've read that Derived Component would solve my problems before, but I can't find a solid example of how that works and apply it to our function.
Editing each foam layer in context, copying objects, and subtracting. I'm exploring that option as well, except I have 7 layers and 6 objects. Thats 42 times I have to do that set of commands. That would be doable if I could subtract the objects from the foam assembly itself, but borderline absurd if I have to subtract them from each layer of foam.
And I have never heard of "Mutlibody solids master modeling techniques".
I will gladly post up the files and would love your help. I just have to make sure that I have nothing in the file thats proprietary first.
Hi RDG3PO,
Would you be able to create the stacked layers in one part file as seperate solid bodies, and then cut them all at once, and then use the Make Components tool to save out the stackd layer as seperate parts?
Make Components
http://www.youtube.com/watch?v=iDRotf2Is2g&feature=share&list=PL35F652F420934D61&index=2
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
If I was starting this project from scratch, I would use a multi-solid modeling approach. However, if I had to retrofit an existing model, deriving would be the way to go. I have attached a simple example of how the derive method would work (at least, one of many ways to do it). Take a look at it, then post back if I need to explain any of the steps I took.
Cameron Whetten
Inventor 2014
@Curtis_Waguespack wrote:Hi RDG3PO,
Would you be able to create the stacked layers in one part file as seperate solid bodies, and then cut them all at once, and then use the Make Components tool to save out the stackd layer as seperate parts?
Make Components
http://www.youtube.com/watch?v=iDRotf2Is2g&feature=share&list=PL35F652F420934D61&index=2
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hey Curtis,
We've tried that function too, and I thought it worked well because we didn't have to predetermine the number or thickness of each of the layers till after the cavities had been subtracted from the whole chunk of foam. We opted to use the "bottom up" method so that we could pre place all the foam layers in a template drawing and have them generate automatically. But that's proving to be fruitless anyway because once I use the Feature Migration tool, it likes to generate new copies of the foam layers anyway, for reasons unknown.
I hate to sound like a broken record, but all my problems would be solved if I could share sketches at the assembly level, sharing part level sketches with the assembly.
Thanks for your help though Curtis, the back and forth has been helpful.
Hey Cameron,
I checked out the files you supplied, and although I was hesitant to click on the file named "thingies", I'm glad I did!
I see how you have all the thingies as one part file, which I understand. Is this a derived component? Some of the placement of the objects in a case is trial and error. Often we have to go back and tweak the location of a component so that it won't interfere with castors, or becasue the cavity needs to be a bit wider, or maybe further away from another component. Would this require making a part file every time the locations of the components were changed?
Also, were the individual layers pre-made as parts and placed into the assembly?
Here's a pack and go of the files I'm working with.
The objects are multibody. The idea is the outer body would be the shape of the cavity, or the envelope of the part. That solid would be hidden once the model was provided to the customer so that they could see their product in th case.
Here is a breakdown of what I did:
1- Create each layer file as a separate file (I really just created one, then saved a copy to get the others).
2- Create the 'voids' file (the one called "thingies"). This is the part that represents the voids in your foam layers.
3- Open each layer part and use the Derived Component command, deriving from the voids file. Derive it as a separate solid body.
4- Use the Move Bodies command to put the voids body into the correct position for that layer (i.e. shift it up or down by multiples of the layer thickness).
5- Use the combine command to cut the void body out of the layer.
6- Put all of the layers into the assembly.
You will necessarily have to modify some of the steps to work with your existing files. For instance, you could instead create the voids part in the context of the assembly, so you could sketch the voids relative to other components. So, if you needed to move them around or adjust sizes or whatever, you could adjust the voids sketch as needed without having to switch to a separate window. Depending on how you do it, the layers should automatically adjust to changes in the voids. It is definitely NOT necessary to create new files every time you make a change to the voids.
The difference between what I just described and what you are doing now, is that instead of creating the voids sketch in the assembly, you would create it in a part, in the context of an assembly.
Post back if you have more questions.
Cameron Whetten
Inventor 2014
Well I have some good news and bad news.
Good news is that dancing the "copy body - combine" jig as described by cwwhetton worked nicely, once I figured out that the process wouldn't work on a sheet metal body. We have our foam layers set as sheet metal features so that our plugin would recognize the foam layers and save them out as .die files for our CNC machine to cut.
Bad news is that the "copy body - combine" jig doesn't work on sheet metal metal parts. Once I've subtracted the parts in place from the layers, I can't convert back into sheet metal. Inventor just doesn't like it.
Again, being able to share sketches and extrude cut at the assembly level would have prevented all the jobbing around. I don't understand why this ability isn't available.
We use the Flat Pattern Extractor from the App Store in order to automate the process of taking all the foam layers in our assembly and spitting them out into a file that our CNC machine can read. The Extractor requires flat patterns, shich can only be made with sheet metal parts.
We're using quite a few iLogic rules in order to generate theinformation we need.Using the Flat Pattern Extractor was nice because we didn't have to pay someone some time to figure out an ilogic rule to do the same thing. I'm sure you can relate though, how aggravating it is that one would have to rearrange an entire workflow just because something seemingly so simple is just not possible in the software.
Can't find what you're looking for? Ask the community or share your knowledge.