Inventor 2018 Professional: mold making problems, doesn't include all features

[Anonymous]

Hey all,

I'm using inventor Professional 2018, on Windows 10.

I'm trying to make a mold for an action figure. I think I understand all the steps to create the mold [extrude block over part. combine cut, the block from the part. split the block and voila, you're mold is done.

However when the mold is created it doesn't include some features, (mirrors) etc.. that where in the original body.

As you can see below is one side of the mold. This is an imprint of the body.

In the original part the abs are mirrored, and clearly visual, however in the mold they dissapear on one side. Even after I keep the original file after the mold cut it is still present in the body, but not in the mold.

Same goes for some other details. But I figure the solution for these problems are all the same.

Any advice is welcome.

Thanks in advance!

[johnsonshiue]

Hi! It is possible the original body has overlapped faces or the Boolean operation went wrong. Please share the files here so forum experts can take a further look. There should be a logical reason to explaining the behavior.

Many thanks!

[Anonymous]

Hey Johnson,

here's the file,

As you can see, when you alter visibility with Solid 2 and solid 25, they differ on various points.
The easiest to see are the abs that aren't mirrored completely.

Edited by Request
Discussion_Admin

[Anonymous]

Or is there a way, to sort of make a part definite. One solid block, with no modifications possible.

That he accepts the part as it currently looks and locks it, and then make a mold of it? Withouth keeping the history of modifications?

I tried saving it as a step file but that doesn't change anything

[JDMather]

Can you Attach your file here?

[Anonymous]

yeah sure

Edited by request
Discussion_Admin

[WHolzwarth]

Though Inventor looks at this warrior's body as a single part, it's not really clean.

There's a protection vest at the left side (looking inside out), consisting of some internal faces (shown in yellow).

IMO this is the cause for the boolean cut error.

[JDMather]

Kudos to @wh for spotting the issue.

The video below is intended to help illustrate the issue.

[Anonymous]

thx you guys already for taking the time and effort to look at this ( @WHolzwarth @JDMather ).  However I'm still not completely following with what a boolian error is, and how I go about fixing this?

I'm fairly new to inventor, so perhaps I'm not designing the right way?

(A litle side note about the neck cut and why it looks like it does. I wanted to create both head and body in 1 freeform part, however as I progressed the file of the 'head part' became to large to modify and proces fluently (to many polygons) so attaching a body to it in one piece would have made my computer explode.

So then I just tried to end the head on a flat surface of the neck. Project geometry those outlines, and from there start a new freeform part to start creating the body. Later on I could then glue these physically when 3D printed, and roughen the small edge up with some sandpaper that was still visible at the neck connection point). Unfortunately this was the best way I could think of..

[WHolzwarth]

You're a very talented guy, Rudy. Congratulations.

I've made some changes, split it by midplane (using the better half), deleted several tiny faces and mirrored back to a symmetrical body. After that workflow like yours.

But be aware, that you've only done a boolean cut. It's not good enough for being a mold, because of some undercuts. You can see these regions after switching Draft1 (Analysis:Draft1) in model browser back to  On.

You need Solid3 set invisible in Solid Bodies(3) for looking into the groove

Before switching you need to pull End of part back down. Moving it up decreases filesize for data transfer

2018 Multibody IPT attached.

Edited by request
Discussion_Admin

[Anonymous]

well thank you , I feel honored getting help from you guys.

it took me a while to figure out the dropping 'End of part' tho, I was looking everywhere to make the object visible.

When I finaly did it crashed Inventor. Tried it again, crashed again. Then dropped 'the end of part' bit by bit, and I only manage to just drop it above where all the "deleted faces begin", to not crash.

I'll try it again now and let my computer process it for some time. Hope it'll work out.

Clever tricke to lower file size tho.

Thanks for making these changes.

Where do i find, Solid Bodies(3) to look into the groove? If you mean, Solid3 in solid bodies(4) then I don't see anything when I make it invisible. And I can't make the other Solid's visible either...?

And how did I create this 'boolian error's?  I'd like to avoid these in the future if possible.

[Anonymous]

Ok now I did manage to get the 'End of part' all the way down, but I'm getting error allerts for most of the deleted faces.

[WHolzwarth · Accepted solution]

Hmm. I downloaded my upload back, and pulled EOP down in only some steps. No error all way down.

What Service Packs are installed? I'm here at 2018.3.4 Build 284

Later: Meanwhile i've seen, that you're using 2018.2 Build 227. Perhaps an upgrade helps

[Anonymous]

I'll try it tomorrow @ a friend who has the 2019 student version.

This is the company's computer and software, and they don't allow me administrator rights.

[Anonymous]

Brilliant! It works on the 2019 version.

Thank you @WHolzwarth it’s much appreciated!

how do I avoid these errors in the future? 

Many thanks again

[WHolzwarth · Accepted solution]

Ok. Now you've seen the same as my model.

How to avoid errors? You can move trogh browser tree step by step from the beginning and watch each result. Sometimes switching to hidden edge display can help, but sometimes it's only disturbing. Moving through sections as displayed about by Jeffrey helps, too. Another way can be using transparent display mode.

For symmetrical models modeling only one half and mirroring later can be good. Faster overall modeling and less failures.

Another way, used already by yourself, is multibody setup and combining back to a solid in a final step.

And last not least: Practicing

[Anonymous]

So basicaly it’s inventor creating these gaps (boolian errors) due to software issues/not updated version. And you just have to check for these occasionaly while modelling in order to not get yourself to much in trouble at the end? 

big thanks to all of you guys for helping me out here 👍🏻

[WHolzwarth]

I don't agree, Rudy.

In this case, most of the problems are made by yourself. Perhaps I can reproduce the differences with Delete Face issues on my notebook, if there's still an old update release present.

Some m9inutes later:

2018.3.4 is installed on my notebook, too.

[Anonymous]

too bad, cause I still don't understand how I created them and how to learn from it for the future?..

[WHolzwarth]

Ok. I'm showing you a first issue, it's not the only one.

Look at the picture below. It's showing irregular geometry in the initial Freeform result (red circles)

These spots are inducing errors. An Extrude to next at one side is not influenced by this issue, but the mirrored feature ends in a bad spot.

In general, extrudes or other features vs non-planar surfaces can result in errors. You can avoid that by extruding with a bit of more thickness than needed.