topic Re: Simplifying Large Imported Step Files in Inventor Forum

Simplifying Large Imported Step Files

jmccollumENV5F — Fri, 20 Nov 2020 22:04:35 GMT

Our company gets a lot of large step files of products from various OEM's; some of them are so large that it makes them extremely difficult to use. We really run into issues when we have to include numerous large step files into one assembly and then export that main assembly for photo sims, thermal testing, etc.

I spend a lot of time trying to simplify these files but it is not a simple process. A lot of the step files are imported as a .ipt file with 500+ solid bodies and the majority of the bodies have large thousands of faces. The file shown in the photos is 193MB. I've tried so many things to compress the files, including exporting all the bodies and creating an assembly file but that still leaves me with a 25MB file that must be transferred between job folders with all the components. To avoid this, I also tried to shrinkwrap the assembly overnight and that just made the file size jump back up to around 100MB.

If anyone has suggestions on what I can do to mediate this, it would be much appreciated.

Re: Simplifying Large Imported Step Files

gcoombridge — Sat, 21 Nov 2020 08:48:27 GMT

I have similar issues with pump motors etc... I derive into a single part (with a single solid) and model over top to reduce detail. Also use the direct edit tools to delete etched text and the 0.2mm fillets bored modellers like to cover their parts with. Still a mission though and time consuming!

Re: Simplifying Large Imported Step Files

SBix26 — Sat, 21 Nov 2020 20:25:07 GMT

I can't determine from your post whether or not you know that you can select which components to import from the STEP file?

My procedure is this for similar complex 3rd party models:

Create new part file
Use Import tool to open STEP file
On the Import dialog box, click the Select tab, then click Load Model (on a very large and complex model this can take a while)
Import displays the model in the graphics area, and the list of solid bodies to be included/excluded in the resulting model (note that if the STEP file is actually an assembly, the component parts will be converted to separate solid bodies)
Select/de-select the bodies to be included (I leave out internal components that make no difference to my design); click OK
Simplify what remains as best I can

If you already do this, sorry for the useless information, but it may help someone else who happens upon this topic.

Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

Re: Simplifying Large Imported Step Files

johnsonshiue — Mon, 23 Nov 2020 19:36:05 GMT

Hi! I believe you will want to delete some of the base features. There are way too many bodies than necessary for your client. Remove all the internal detail bodies (deleting the features). If some of the geometry is critical as locators, replace it with work geometry or a UCS.

Many thanks!

Re: Simplifying Large Imported Step Files

jmccollumENV5F — Mon, 23 Nov 2020 20:48:24 GMT

@gcoombridge

Yes, it seems like you feel my pain! I don't see the option to import the .stp as a single body. Do you use the combine feature once you have opened the part? We really only need the external profile as well but it does need to be accurate because we are fitting this equipment in tight enclosures and running thermal simulations where the profiles of the heat sinks are important.

I haven't found a good way to simply derive the external profile because there are small ±.1mm gaps between a lot of the parts so patch/sculpt is not very effective if I have multiple parts in one single body. If I export the bodies into an assembly and attempt to shrinkwrap while filling the internal voids, the gaps present the same issue.

I try to remove unnecessary faces/fillets and 3D text on the bodies when possible. I have also tried messing around with composite surfaces but I am no expert with those. Anything else that I may be missing and have helped you in the past?

Re: Simplifying Large Imported Step Files

jmccollumENV5F — Mon, 23 Nov 2020 20:50:54 GMT

@SBix26

It's not useless information! It would've helped me when I first started trying to simplify these files. My typical workflow is very similar but slightly different as I will import all of the bodies into the 'master' .ipt file and then create a separate 'simple' .ipt where I delete any solid bodies that are not necessary.

It is just easier to do with the large files since it is hard to sort through SolidXXX one by one and it also allows me to rename the important solids/features so I know what is what. It also gives me a good starting point if I need to use the 'master' .ipt to create a different 'simple' .ipt.

The file sizes should be comparable in both methods (selective import & 'simple' ipt), correct? Or does originally importing all the bodies leave some sort of trail within the file that increases it's size, even after the bodies/features are deleted?

Re: Simplifying Large Imported Step Files

jmccollumENV5F — Mon, 23 Nov 2020 21:20:54 GMT

@johnsonshiue

I am importing these step files from other companies. Without getting too specific, the files we receive is of very new technology from large corporations and we aren't able to really request simpler .stp files to use as they don't want a lot of the confidential design info getting passed around.

I attempt to remove all the internal bodies from the original .stp file and then remove 3D text and internal cavities from the individual bodies to try to simplify them. The faces are not always clean though so deleting faces/features can get pretty complex. In the attached photo, I cannot delete/heal the faces on the 3D text & angle markings because they are not clean. Even after repairing geometry, it would not heal because of how the faces intersect.

Re: Simplifying Large Imported Step Files

jmccollumENV5F — Mon, 23 Nov 2020 21:34:40 GMT

All, here is an example of one solid body that comes in through the main .stp file. There are typically 5 or so parts with this complexity out of the 500+ imported solid bodies.

The external profile with the heat sinks is needed but the profile with the internal cavity is not needed. Even when I try to patch/sculpt or delete/heal faces of the 3D text or internal cavities, it doesn't affect the file size in a very efficient way.

Re: Simplifying Large Imported Step Files

WHolzwarth — Mon, 23 Nov 2020 22:42:56 GMT

Here's a startup, using some sculpts. STEP in Zip attached, IPT is about 21.5 MB.

Re: Simplifying Large Imported Step Files

WHolzwarth — Mon, 23 Nov 2020 22:46:16 GMT

Well, this forum always is a mystery to me.

I've tried adding a second picture by editing my first message, but no luck.

Here we go

Re: Simplifying Large Imported Step Files

gcoombridge — Tue, 24 Nov 2020 01:24:14 GMT

@jmccollumENV5F

I would typically import the step file (which will come as an assembly), save this and then derive into a single part combining the solids at that point. Sometimes this does make a larger file than having a multi-solid part. If I have the option on an online portal I will always download .SAT files because they can be turned into a multi-solid on import.

There are lot's of options for reducing the geometry but don't discount simply extruding over top of it! Have a look at the attached images I sent one of my colleagues as an example...

Re: Simplifying Large Imported Step Files

johnsonshiue — Tue, 24 Nov 2020 22:14:09 GMT

Hi! On top of experts' comments, I think there are plenty of opportunities to simplify in your case. Sometimes, it might be quicker just to recreate the geometry with simple cylinder or box. Your client may not care about the fillet and the detail faces on the motor. But, the mounting holes and rough size may be important. You can easily get the mounting holes by creating workaxes and workpoints. Then you can use Delete Face -> Lump to remove the motor body. And, recreate it using simpler geometry.

Many thanks!

Re: Simplifying Large Imported Step Files

Mark-Jackson — Tue, 06 Dec 2022 00:16:40 GMT

I have found that simply importing and then exporting into 3ds Max reduces STEP files by 60 - 75% . If you run the Weld command in 3ds Max to join adjacent geometry together you get another significant reduction. Frequently a 500000kb step file will reduce to 50 - 75000kb with just those two steps and without any detail loss. If you need more then 3ds Max Pro-Optomizer command can reduce the file down to 5-7000kb but with losses in detail.