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Switch from SolidWorks to Inventor iLogic and iPart Help

8 REPLIES 8
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Message 1 of 9
stretchoranamo
3314 Views, 8 Replies

Switch from SolidWorks to Inventor iLogic and iPart Help

Hello,

 

First off let me start off by saying I am very new to Inventor, but have used SolidWorks extensively for many years. 

 

I apologize first off if this subject has been covered (I have been searching forums and YouTube for some time), and for my lengthy post.

 

We are looking to switch from SW to Autodesk in order to utilize advanced surfacing in Alias, and its interoperability with Inventor.  However, we need to continue to perform Kinimatic linkage studies as well using Inventor.  I need to make sure we can perform the same calculations with ease before making the switch.

 

At this point I am trying to mimic in Inventor the kinimatic studies I perform in SW.  In SW I would perform these studies within a single part file, using a single sketch only (no solid parts).  Within this part file I would break up the total "travel" of the linkage into configurations that are driven by a "Design Table".  The Design Table would be used for both the main driving value, and for any driven values I wanted to use for analysis.

 

I am trying to find a way to get the same driven variables written to an Excel file to use for analysis using Inventor.

 

As a test example:

 

I would like to drive one variable(Damper Length) to get ~20 different iParts, each with the linkage moved to a new point within its set range of motion.  I then would like to write several Driven variables(Displacement_1-3 shown in "RULE CODE" attachement) from each iPart instance to an Excel file.

 

I have been able to get my 20 iParts and the linkage to move accordingly(iPART INSTANCES attachement), but I have not figured out how to write the driven data to excel for each iPart instance(20 rows of data, 3 columns).  I have only been able to write the dimesions for one row of data...whichever iPart is currently open.

 

Can anybody help with the necessary iLogic code or another solution?  It seems like this should be pretty straight forward.  Do I need to be using the "ChangeRow" iPart Snippet?

 

If anything is not clear please let me know.

 

Thanks a lot in advance for any help.

 

Cheers

 

 

 

 

8 REPLIES 8
Message 2 of 9

Hi stretchoranamo,

It sounds like you're on the right track here. I'll try an work out an example and confirm that "ChangeRow" is indeed the correct way to do this. I'm thinking that we might have the code write to an array for each ChangeRow, and then write the array values out to the Excel file. Also, kudos to you for the clear description of your goal and the screen shots, that helped with understanding the questions.

 

Depending on the amount of time I find, you might work this out on your own first. If so, I just wanted to point you to this forum where  you can search and ask programming questions of this type  too:
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/bd-p/120

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 3 of 9

Hello Again,

 

I have decided to re-phrase my question to make it simpler.  I also wanted to mention that I am very new to any sort of programming as well, and have been trying to learn by example.

 

SETUP

 

I have setup a single sketch within a part file.

 

4-bar linkage sketch with a damper.  I would like to break down the travel of the damper into 21 instances and anylize the motion of the linkage.

 

1 driving dimension  :  DAMPER_LENGTH

3 driven dimensions:  DISPLACEMENT_1, DISPLACEMENT_2, DISPLACEMENT_3

21 iPart "Instances" 100, 101...120 in which the "DAMPER_LENGTH" varies from 85mm to 65mm in 1mm increments

 

Please see the attached file "SETUP" for an overview

 

WANTED FINAL OUTPUT IN EXCEL

 

Please see the attached file "FINAL EXCEL FILE".  I would like to use iLogic in order to write and Excel file as attached.

 

I would would like to include logic to "re-run" through all 21 instances and then output the file.  This way I get new data for all instances if a change is made to any of the geometry.

 

I need help writing this code.

 

Thanks again.

 

 

 

Message 4 of 9

Hi Curtis,

 

Thanks a lot for the reply, I really appreciate it. 

 

Also, noted that there is a specific location within the forum to ask programming questions.  I will post further questions of this nature there.

 

I re-phrased my quesiton and posted some new images to make my question more clear (I was working on this new post while you replied and did not notice).  I will also post the .ipt file. Do you mind taking a look when you get a chance?

 

Cheers

 

 

Message 5 of 9

Hi stretchoranamo,

 

I wonder if you can do this without the need for iLogic by exporting the driven dimensions as custom iProperties, and pulling those into the iPart table, as shown in this illustration. Once in the custom iProperties are in the table, then you can just switch rows in the model to set the driven dimension iProperty for each row (select Yes when asked to update the table).

 

Once this is done you can edit the table as a spreadsheet to get the values.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

Autodesk Inventor iPart Table.png

 

 

Message 6 of 9

Awesome, thanks for the quick reply Curtis.

 

I did not realize that you could grab parameters to use within iPart like that.  This will be very helpful.  Attached is the part file with your recommendation if anyone else finds it useful.

 

A couple of questions:

 

1.  Is it possible to get the driven values without the "mm" in Excel?  Or is using an excel function the best option to start using the as numbers to analyze?  See the attachment "MM REPLACE"

 

2.  To continue the discussion further, is there a goodway to automate this process either through this method, or with iLogic (Or maybe a Macro)?  I understand if Curtis does not have the time to go further into it.  I imagine that one could program a solution to speed this process up and I would love to get some recommendations.

 

During the deisgn process many geometry revs will be performed and then the driven values will be recalculated and analyzed.

 

It is actually pretty time consuming (and there is the potential to make a mistake and not click every row) to use the suggested solution.  After each row is clicked I get a warning to say "Yes" to so that the table is updated (See attchment "WARNING_MESSAGE").

 

Ideally I would make a geometry change, run a Rule/Macro, and in turn get the updated spreadsheet.

 

Thanks.

 

 

 

Message 7 of 9

Hi stretchoranamo,

 


stretchoranamo wrote:

1.  Is it possible to get the driven values without the "mm" in Excel?  Or is using an excel function the best option to start using the as numbers to analyze?  See the attachment "MM REPLACE"

 


In the Parameters editor, right-clck on the driven dimension and choose Custom Property Format, then uncheck the Units String checkbox.

 

I try and revisit question 2 later.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 8 of 9

Great, thanks!

These tips are so helpful when learning new software.

Looking forward to your reply to question 2 if you get around to it.

Cheers
Message 9 of 9

Hi stretchoranamo,

 

I'm stuck working late, and just looked in on this thread.

 

To avoid the "WARNING_MESSAGE" about the row value change, I think (if I recall correctly) you can change a setting to set the edit focus from the iPart factory (the parent) to the member (the child / row). This link speaks to this setting for iAssemblies, but you should be ablt to do the same for iParts (assuming I'm remembering correctly):

http://beinginventive.typepad.com/being-inventive/2013/05/adding-multiple-components-in-iassembly-ta...

 

Also, I wonder if the Autodesk Force Effect application is of any interest or use to you?

http://youtu.be/sRn80DA8cx8

http://www.cadlinecommunity.co.uk/News/NewsItem.aspx?NewsItemId=c8b90344-0e6b-47b6-8888-fd749b8d4868

https://chrome.google.com/webstore/detail/autodesk-forceeffect/ekbaidcchahkpedbhdenlmleimihkcim?hl=e...

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

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