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I can get a computer that's less than a year old which would barely be useful for our receptionist, let alone 3D work. So actual specs would be a good start, including Inventor version, OS version, input devices (3D mouse, for example). Some idea on part counts/complexity would also help.
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If you are going to fly by the seat of your pants, expect friction burns.
"I don't know" is the beginning of knowledge, not the end.
If you are going to fly by the seat of your pants, expect friction burns.
"I don't know" is the beginning of knowledge, not the end.
@Anonymous
In addition to @dgorsman request for additional information here are some other things to consider
Disable your anti-virus application on 1 machine and see if that changes the performance. If it does, apply the necessary exceptions
Clean out your C:\Temp, C:\Windows\temp, and your C:\Users\[username]\Appdata\Local\Temp folder. Appdata is a hidden folder and you may need to adjust your viewing settings.
Perform a disk defrag (unless you have a SSD drive). It may be necessary for you to clean up your hard drive and repair registry. Use a tool like CCLEANER (but at your own risk).
Turn off Windows Bells & Whistles, use classic theme, and disable desktop gadgets and unused (Windows) services.. Also configure Inventor and Windows per the recommended performance options (Review this and that)
If possible keep Inventor Design Data locally. Having it on the network can lead to performance issues.
Work locally on your models if possible. If you have to store your models on the network. Leave the common files on the network and move your models back and forth using a file management tool. May want to consider implement Vault basic..
Keep your sketches simple and only project the necessary geometry.
Resolve issue via the Design Dr. Don't ignore them. Every so often on your model, perform a rebuild all. Other things to consider, limit adaptivity and use modeling functions over sketching commands. If you need to use the adaptive method.. Use it and then turn it off when done.
I know this is common sense, but keep your workspace, hard drive, or share network location organized and clean.
Properly configure a project file. Define the workspace and etc.
Don't put your eggs all in one basket when it comes to assemblies. Demote, simplify or break your model up into smaller chucks, Use the BOM structure to your advantage.
Simplify, Simplify, Simplify. Determine if the exact details are really necessary. If it is, create a simplified version (iPart, derived, shrinkwrap and etc) of the part. Think about using appearance over detail
Review the Autodesk Inventor 2014 working with large assembly performance guide
Unload unnecessary Inventor add-ins
Invoke defer update and manually update when you're ready.
Look at creating View Reps, Level of Details (LODs), or working with Express Mode with your models.
Thinking about using the drawing open options to defer updates/fast open
Switch drawing view preview to partial or boundary box (Tools/Application Options/Drawing tab)
Think about the parent to child relationship. Do you have these options turned on in Application Options (Relationship redundancy analysis and features are initially adaptive) ?
Are you putting too much details in your drawing.. Like trying to jam 20lb worth of stuff in a 5 lb bag.. Break up your drawings into smaller chunks.
Constraints consume memory. Simplify them as much as possible. Maybe you want to ground your components or consider using skeleton modeling techniques. Or suppress constraints to limit them if you have numerous ones.
IF you're using bolted connections, this can impact performance. Create LODS and turn them off when not needed.
Set your Windows Virtual Memory to the recommend settings.
Make sure your graphics card driver is up to date. Don't rely on Windows telling you it is. Go directly to the Vendor web-site.
If you're using the 3D Connexion device.. Make sure its driver is up to date and you have calibrated it.
Limit the number of other Windows application that are currently running.
Use the "Disable Refinement" option if you're using Inventor 2016 or newer. (This option is located under Tools/Application Options/Display tab)
If you are using shaded views in your drawing, try to limit them because they too will impact performance. In Document Settings/Drawing tab, make sure the Shaded View/Use Bitmap option is set to Always.
In Tools/Application Options/Display tab, you may want to consider setting Min Frame rate (Hz) to zero. Thus allowing faster rotation/spinning/orbit of your model.
Yes there's a lot of info here and not everything I pointed out will work for you or for others who may review this information. But its another way of looking at boosting performance in your model
Mark Lancaster
& Autodesk Services MarketPlace Provider
Autodesk Inventor Certified Professional & not an Autodesk Employee
Likes is much appreciated if the information I have shared is helpful to you and/or others
Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
I've attached one file that may help, I'll try and track down a couple of other documents.
Have you also looked at using "Express View"?
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
@Anonymous
Yes it is.. 
That's why I always finish with "Yes there's a lot of info here and not everything I pointed out will work for you"
Actually I'm presenting a class at AU2017 regarding this very same topic... "Boosting Inventor Performance" if anybody is interested in learning more about this topic and attending AU..
Mark Lancaster
& Autodesk Services MarketPlace Provider
Autodesk Inventor Certified Professional & not an Autodesk Employee
Likes is much appreciated if the information I have shared is helpful to you and/or others
Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Hi! The hardware spec looks fine to me. How large is the assembly? Could you share the files with us to understand the behavior better? Do you have access to Inventor 2018?
Many thanks1
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi! Purely based on the file size, it does sound large. But, we have customers working on drawing and assembly equivalent or larger than the one you have with good performance. Something does not make sense to me. You mentioned that you have files stored in network drive. Is this a network drive on your domain? How far is it from your machine to the server?
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
@Anonymous wrote:
Another co-worker thought maybe I should be using Plant 3D to build my assembly...???
That depends on a number of factors. It doesn't handle detailed work as well as Inventor, it's much more "macro" in scale using simplified components and specification-driven selection. If you need to follow "piping specs", require "piping iso's", and care more about pipes and valves rather than individual nuts'n'bolt types and locations, Plant3D may indeed be a better choice. If you are doing primarily mechanical design, with piping components only part of the model, and parametric controls are necessary, you'll want to stay with Inventor.
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If you are going to fly by the seat of your pants, expect friction burns.
"I don't know" is the beginning of knowledge, not the end.
If you are going to fly by the seat of your pants, expect friction burns.
"I don't know" is the beginning of knowledge, not the end.
Not really unless you are the only person using Inventor. Generally Pack and Go is used to get a copy of files of a specific assembly to send to someone and not an everyday work process.
With the improved results by bypassing the network, it shows where your issues are, in this case your network. It's a good indication that you have issues with your network, either server(s) or switch/router(s).
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
@Anonymous I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!
About Packaging Files with Pack and Go
Using Pack and Go with Autodesk Inventor
Please select the Accept as Solution button if a post solves your issue or answers your question.
Kelly Young
* Ideas * Help * AKN * Updates * Pack & Go * Reset Utility * Repair Install * Customization * iLogic Examples * Autodesk University *
Hello together,
Please work with LOD and replacement objects for assamblies.
Only this works, we work with assemblies up to 80,000 parts, with replacement objects and LOD, it is 2500 parts.
Please see the Video.
Please the computer test >>> Test <<<
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