Getting ipart length into part number and file name from a driven dimension

[HO-AD]

Hi all, I have a derived ipart factory that is based on a vessel template and uses other criteria (angle, tangental offset, inside & out projection) to determine the nozzle placement and length. I have a driven parameter that is the overall lenth that I'd like to display in my part numbers and file names but I cant get it to work properly. I exported the parameter as a custom iproperty but on the table, the lengths for the various nozzle sizes all match the master ipart length.

How can I get this to update properly for each size when I place them?

Thanks, Paul

[Curtis_Waguespack]

Hi HO-AD,

ipart members do not have their own iProperties. So that approach won't work, as you noticed.

You'll want to use the length Parameter in your file name and part number directly. To do so you can use Excel to concatenate your strings, as shown in this example (in this example it uses description instead of part number or filename):

http://books.google.com/books?id=c7xtaUHf_m0C&pg=PT500&lpg=PT500&dq=curtis+waguespack+ipart+descript...

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

[HO-AD]

Thanks Curtis but I have already been trying this using formulas in excel. Here are some pictures that might help explain.

This first one shows that I'm using the highlighted driven dim and a user parameter for "NL" (my length)

Here I made it a custom parameter and inserted it into the table

Here shows my expression containing NL

Next 2 pics show the part inserted into my assembly with the desired internal and external projection w/ the wrong length listed in the part number

Custom parameter shows true length.

This also happens when I insert the parameter into the table directly from the parameters tab except it shows up "d130 + IP" in all my members

[Curtis_Waguespack]

Hi HO-AD,

Thanks for providing the detailed information and screen shots.

I see the issue now. The wrinkle is from the "d130 + IP" value. I would suggest doing that computation again in Excel, and then using that column in the Part Number and FileName expression.

One tip that you might or might not be aware of already, is that if you create an empty column in your speadsheet (one with no header) you can then have other columns to the right of it that the iPart table won't read.

So I would pull d130 and IP into the table, and then edit the table in Excel, then skip a column and create a new column called NL and create the expression. Then use the NL column in your excel formula for the PartNumber and FileName columns.

The issue with this method that you need to be aware of is that if you change the NL dimension so that is no longer "d130 + IP", then your spreadsheet needs to be updated too. So it's not a perfect solution, but I've used this method many times in the past.

Edit:

I should point out also, that for your solution you don't really need to leave a blank column in the spreadsheet. If you choose not to the NL column will simply show in your iPart table colored in red, to indicate that it has a forumula calculated in the spreadsheet. But I often use the blank column trick to hide messy extra columns that are created just for doing some calculations or formatting.

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

[HO-AD]

Thank you Curtis it seems like I'm almost their.. But I have one more issue. I cant find d130 in the parameters tab of the ipart authoring pane. Is this because it is driven dimension / reference parameter? Are driven dimension / reference parameters not allowed in the table for some reason?

[Curtis_Waguespack]

Hi HO-AD,

I think you've stumped me.

I've run into this in the past and don't think I ever found a solution or acceptable workaround.

Autodesk's thought (intent) on this is that purpose of iparts is to configure parts and features that we modify directly by updating dimensions, and since the driven dimensions cannot be modified "directly" we are not given access to them in the iPart table.

If I recall correctly, in the past when I ran up against this I had to change my dimensioning, sketching and / or modeling approach to get the information that I needed into the iPart table.

I've created an improvement idea on the Inventor IdeaStation to bring attention to this issue:

http://forums.autodesk.com/t5/Inventor-IdeaStation/Allow-Driven-Dimensions-to-be-used-in-an-iPart-ta...

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

[HO-AD]

Well dang. I appreciate all your help Curtis. I guess back to the drawing board it is. If I was proficient in ilogic and vba I'm sure I could find another way to go about what I'm trying to do ultimately. I guess back to the books it is!

Thanks again for your help Curtis! Your book has been invaluable to me.

[ADSKDJW4]

As Curtis has already commented on this, this cannot be achieved at this time. since its been entering to Ideas station it hopefully will be reviewed and potentially incoporated into a future release.

Regards,

Don

[rianm]

Good day,

I am in the process of creating my own steel library, including my own custom profiles and SA Steel sizes etc. Which will then anable me to use this library in the frame generator. There is only one problem, the length of the Ipart does not update in the part number/filename once used in frame generator? I have been through countless links on the internet and just cant find the solution.

Will anybody be able to assist me regarding this matter?

Thank you.

[Mark.Lancaster]

In frame generator the members (file) name is automatically assigned as the standard+designation column+a sequential number.  For example ANSI 2x2x1_8 00000001.ipt.

However you can manually change it by selecting the prompt for file name or have a program do that for you.   In regards to the part number it is based on the version of Inventor you have.  I think in Inventor 2015 (maybe it was 2014) you have the ability to pull the part number that is defined in content center, however prior to that Inventor defined the part number based on the file name.