Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Inventor 2014 Express Mode

16 REPLIES 16
SOLVED
Reply
Message 1 of 17
graeme.robinson
2135 Views, 16 Replies

Inventor 2014 Express Mode

Hello

 

My memory is failing me...

 

Express Mode, this makes the file size larger? or was that another feature?

 

If so, how do I dentify which assemblies have had the express mode size inflation applied to them?  

 

Thanks in anticipation

 

Graeme

16 REPLIES 16
Message 2 of 17
mcgyvr
in reply to: graeme.robinson

Frankly the autodesk documentation for what express mode is just "sucks".. 

I can't tell what it really even does.. 

There are a few blog posts about it though..

http://enceptia.com/inventor-2014-large-assembly-performance-is-no-joke/

http://www.cadlinecommunity.co.uk/Blogs/Blog.aspx?ScoId=1a78bf7d-dc3b-4af7-afda-49b2b3f1c31b



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 3 of 17
graeme.robinson
in reply to: mcgyvr

Thanks for that

 

yeah there is little information.....

 

I seem to remeber when I went to 2014 seminar they were saying how great it was, but also mentioned that if made files much larger......

 

Thanks

 

Graeme

Message 4 of 17

Graeme,

 

By Default, any assembly which references more than 500 files will have Express data written to it when saved in 2014 or 2015. This number is configurable from the Assembly tab of App Options.

 

How do you tell ? Well I must admit I usually just sort by filesize at the OS & then it's obvious since Express data will typically make the .iam file at least 10x bigger. You can also hit the Options button after picking an iam file from the File open dialog; if Express data is present then the option to use it will be checked. I'm not aware of an iProperty that shows this though.

 

Once an assembly is open in Express mode, the most obvious way to know this is that the ribbon contains an icon called "Load Full"; ie unload Express data & load the full fidelity data. Also the assembly browser will show a badge at the top which states Express view.

 

If you don't want to use Express mode then you can uncheck the option from the Assembly tab on App Options & resave the assembly & the data will be removed.

 

Note that the initial open & graphics interactivity/performance is considerably imporoved when working in Express mode.

 

Hope this helps,
Chris



Chris Mitchell
PDMS Customer Engagment Team
Autodesk, Inc.

Message 5 of 17

Chris

 

Thats great thanks for the concise and helpful information

 

Ill trawl through the vault and find the offending huge assemblies and de-express them

 

The files are big enough without having them 10 times bigger and we have the hardware to cope with the fully loaded assembly

 

also worries me that since all assemblies have sub assemblies worked on by different teams that opening in express mode could in theory show out of date graphical data.....I've been caught out before with that happening in Solidworks a long time ago..

 

Again, thanks for you help

 

Graeme

 

 

 

 

Message 6 of 17
mcgyvr
in reply to: ChrisMitchell01

Chris,

Is there a "GOOD" description somewhere of what "express mode" really is/does.. what it effects.. why one would suggest turning it on, what problems on could have with using it, etc... ?

I've found VERY little information other than "hey users we now have this wonderful express mode".. 

 

I'd love faster large assembly performance but don't know if its going to cause problems or stop me from doing something or make me lose something or what...

 

I'm finding a bit of info now.. Like it disables some assembly tools.



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 7 of 17
ChrisMitchell01
in reply to: mcgyvr

Graeme - Your concern about the "cached" Express data getting out of sync with lower level part changes shouldn't occur based on the way we check for those sorts of things - if you have actual examples of that happening then please do let us know.

 

I've also asked one of the Sr. software developers to add some additional technical supporting information, here (likely tomorrow). Also an internal document relating to working with large assemblies should be accessible from an existing support knowledge article by tomorrow too.

 

Thanks,
Chris



Chris Mitchell
PDMS Customer Engagment Team
Autodesk, Inc.

Message 8 of 17

Chris

 

Youve got me intrigued....

 

how does this cached data then update when other lower level sub assemblies have been updated without the top level assembly being opened?

 

Its more the file size thats the issue we make our IT infrastrucure must bigger or just wait a little longer for a file to open?

 

Thanks again for most useful information

 

Regards

 

Graeme

Message 9 of 17

Hi Guys,

 

Thanks for all the questions and feedback. I have attached an addendum document describing express mode functionality in detail - I have tried to highhlight the most important aspects of express mode. You can refer to the information in there to help you choose what workflow works best for you. 

 

I have tried to address some of the questions posted here in that document......particularly look at the section talking about "Edit Scenario" and "File Size Considerations".

 

Feel free to post back with questions or send me and Chris an email directly. You can reach me at sundarsATautodeskDOTcom

 

Thanks

-Shiva Sundaram

Inventor Engineering

Autodesk, Inc.

Email: sundarsATautodeskDOTcom

 

Message 10 of 17

Thats fantastic....consise and to the point

 

Would it be not worth mentioning typically how bloated the assemblies get?

 

From a Vault Administration point of view this is very important..

 

But I am being picky....

 

Great stuff

 

Thanks

 

Graeme

Message 11 of 17

Hi Graeme,

 

Good question on the file size increase. The file size increase is not something we can predict easily. It depends on multiple factors like

 

a. number of unique parts in the assembly

b. number of instances in the assembly

c. geometric complexity of part (analytic surfaces, splines etc).

d. whether or not the part has enhanced tessellations

e. materials / colors used

f. graphics settings / device / graphics card

 

So, the answer is - it really depends. You might want to do some sampling with your datasets to see how much the increase is and average it out. In general, on an average, I would say it could vary anywhere from 2X to 4X of original file size for average assemblies but we we have also seen bigger increases for extremely complex assemblies. So, it really varies.

 

If you are concerned about vault, then the best thing would be to purge the assembly of the express data for all intermediate revisions and save the express data ONLY on the final revision. That way you would minimize the storage impact.

 

Thanks and keep the questions coming 🙂

 

-Shiva Sundaram

Inventor Engineering

Email: sundarsATautodeskDOTcom

  

Message 12 of 17

A quick question to add: how do iProperties interact with Express mode?

 

Are the iProperties of sub parts refreshed when opening in express, or will they be out of date and require a manual update?


--------------------------------------
Did you find this reply helpful ? If so please use the 'Accept as Solution' or 'Like' button below.

Justin K
Inventor 2018.2.3, Build 227 | Excel 2013+ VBA
ERP/CAD Communication | Custom Scripting
Machine Design | Process Optimization


iLogic/Inventor API: Autodesk Online Help | API Shortcut In Google Chrome | iLogic API Documentation
Vb.Net/VBA Programming: MSDN | Stackoverflow | Excel Object Model
Inventor API/VBA/Vb.Net Learning Resources: Forum Thread

Sample Solutions:Debugging in iLogic ( and Batch PDF Export Sample ) | API HasSaveCopyAs Issues |
BOM Export & Column Reorder | Reorient Skewed Part | Add Internal Profile Dogbones |
Run iLogic From VBA | Batch File Renaming| Continuous Pick/Rename Objects

Local Help: %PUBLIC%\Documents\Autodesk\Inventor 2018\Local Help

Ideas: Dockable/Customizable Property Browser | Section Line API/Thread Feature in Assembly/PartsList API Static Cells | Fourth BOM Type
Message 13 of 17
sundars
in reply to: MechMachineMan

Hi Justin,

 

iProperties are not affected by Express workflows. They do not need to be refreshed and always reflect their current state. So, if you change a sub-assembly or part's iProperties, then open the top-assembly in express mode, any iProperties you retrieve from those subs or parts will always in their current state (i.e. last saved state).

 

Thanks

-Shiva Sundaram

Shiva Sundaram
Inventor Development
Message 14 of 17
MechMachineMan
in reply to: sundars

Another question for you:

 

Is express file data saved at a different time then full load data?

 

Issue I am running into:

- Moved files.

- Reference becomes broken in model

- Load model as express, fix reference

- Click to load full, save model.

- Close model.

 

- Run code that opens the same assembly with options, to open it in express mode

- Code runs into issues about not being able to resolve the file.

 

Does this imply that express mode data is only saved when you first enable express mode, and then again when you save WHILE in express mode, and not if you save during full load?

 

Thanks again!


--------------------------------------
Did you find this reply helpful ? If so please use the 'Accept as Solution' or 'Like' button below.

Justin K
Inventor 2018.2.3, Build 227 | Excel 2013+ VBA
ERP/CAD Communication | Custom Scripting
Machine Design | Process Optimization


iLogic/Inventor API: Autodesk Online Help | API Shortcut In Google Chrome | iLogic API Documentation
Vb.Net/VBA Programming: MSDN | Stackoverflow | Excel Object Model
Inventor API/VBA/Vb.Net Learning Resources: Forum Thread

Sample Solutions:Debugging in iLogic ( and Batch PDF Export Sample ) | API HasSaveCopyAs Issues |
BOM Export & Column Reorder | Reorient Skewed Part | Add Internal Profile Dogbones |
Run iLogic From VBA | Batch File Renaming| Continuous Pick/Rename Objects

Local Help: %PUBLIC%\Documents\Autodesk\Inventor 2018\Local Help

Ideas: Dockable/Customizable Property Browser | Section Line API/Thread Feature in Assembly/PartsList API Static Cells | Fourth BOM Type
Message 15 of 17
sundars
in reply to: MechMachineMan

Hi Justin,

 

If your express mode is enabled we will save express data whenever you save the assembly file regardless of whether the assembly is opened in express or full. We only save express data on the active assembly document being saved (i.e. only top assembly). If some child sub-assemblies are being saved along with the top, we do not save express data for those.

 

We do not save anything during Load - during load we only load express data if you have specified the Application options to load express data when opening an assembly.

 

Express doesn't break any file references. If you have moved any files out of the project or removed them from your file search path and the next time you open the assembly referencing those files, you will be prompted to resolve (and this will happen for both express mode open and full mode open). 

 

In the file dialog, if you click on the assembly you are about to open and click on the options button, it should show you an options dialog where you can specify your open options (open express, design views, pos-reps, lods). At the bottom there is a checkbox which says "Skip all references". If you check that you will not be prompted to open the referencing document.

 

Can you elaborate your steps on what you are seeing - You can also send me the dataset if you like and I can take a look - you can email me at "sundarsATautodeskDOTcom"

 

Thanks

-Shiva Sundaram

 

 

 

Shiva Sundaram
Inventor Development
Message 16 of 17
smokes2998
in reply to: sundars

2014 express mode is very limited in functionality. (It is a really  bad copy of  SW light weight assemblies)

If you want to do any  work with the assembly you have to switch from express mode to full mode. Switching can take just as long as loading a full assembly.

 

 

Message 17 of 17
sundars
in reply to: smokes2998

Hello,

 

2014 was our first release of express mode and there was only so much we could fit into it. In 2015 we enabled more functionality like Edit-in-Place and other create workflows. 

 

Another reason why we disabled many workflows was that they would invariably invalidate the lightweight-ness of the express assembly. However, we are continuously re-evaluating express mode workflows and if you have any suggestions or requests on functionality that you need for enabled please let us know.

 

You can reach me directly at "sundarsATautodesk.com" with your requests. I will make sure that it gets reviewed by the team.

 

Thanks and Best Regards

-Shiva Sundaram

Shiva Sundaram
Inventor Development

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report