Through my searching I have found that if I want to get my flat pattern extents dimensions in the parts list I create custom iProperties with the following entries:
=<SHEET METAL WIDTH>
=<SHEET METAL LENGTH>
This gives me what I am looking for, almost. The values given are in decimals of an inch and I need them fractional. Normally we do this through the use of parameters with custom property formats. The trouble is, I don't know how to get these properties (the SHEET METAL WIDTH, etc.) into a parameter where I can export them the way I need them. Can someone shed some light on how to do this or where these sheet metal properties even come from?
Thanks for the help again.
Solved! Go to Solution.
See this thread for some help http://forums.autodesk.com/t5/Autodesk-Inventor/Fl
You can find an unsupported add-in to add parameters for the properties.
Please be aware that adding parameters for Flat Pattern extents can cause cyclical dependencies
(that's the reason why the extents are not available as parameters). Use the add-in at your own risk!
You just need to take it a step furthur. What name did you give your Custom iProperties?
In you Parts List use the Column Chooser and create a new Property that has the EXACT SAME NAME as the custom iProp.
Then you should get them to show up in the Parts List. Right click on the column in the Edit Parts List Dialog box and choose Format Column. Go to the Apply Units Formatting and select Fractional Format. You should be good to go.
You might also have a look at iPropWiz (www.ipropwiz.com). It handles this without the need for creating parameters and is more flexible than the parts list only solution. Plus much other property goodness.
Thank you all for the responses. The last few posts I put up got nothing from everyone and I was starting to think I was blacklisted somehow . Anyway, Mark's answer gave me a workaround for my project that I needed but unfortunately it isn't a permanent answer. Most of my assemblies have 15 or so parts and only one out of about 100 have a sheet metal component to them. To have two more columns in my parts list for just the one part looks a little odd (I have yet to even hear what the client thinks), but it did work and I thank you for it.
It looks like ipropwiz is the way to go for this kind of thing. I'll have to do some more research and then give it a go.
Thanks again everyone.
You lost me on this one a bit. Why do you need to call a flat pattern parameters in the parts list on the assembly drawing? I would say that the info belong to the drawing of the individual part. To my way of thinking Mark has pointed you to the right direction.
There is one small thing to add in regard to the dimension units. Here is a copy of a reply from RobV:
From: "RobV" <email@example.com>
Subject: Re: IV2009 sheet metal extents in Parts List ?
Date: Tuesday, 29 April 2008 4:21 AM
"There is a workaround to get the length, width, and area in, but in my
opinion could have been made better:
In your sheetmetal template, in custom iprops, create a new property whose
type is Text and the name can be anything. For the value use one of the
= < Flat Pattern Area > cm
= < Flat Pattern Length > cm
= < Flat Pattern Width > cm
Initially the value of the property will display as the expression string
but clicking Apply will change it to the actual value of the other property.
You can now use these in the BOM as custom properties. (The cm MUST be
there as Inventor uses this native unit to properly do all of its
conversions.) You can then pull in each of the text properties to your
Thanks to Brian Ekins, Seth Hindman, and Lucia Casu for pointing these
Inventor 2008 SP2
Why do you need to call a flat pattern parameters in the parts list on the assembly drawing?
I apologize but you may want to get a fresh cup of coffee because this is about to get insanely "wordy". I'm just not sure I can sum this up any easier without just making things worse.
One of the six services my company provides is fabrication drawings for the industrial steel fabrication industry. These fabrication practices are governed by AISC and NISD guidelines and codes where I am located in the US. This industry has adopted practices that are followed by most of the steel fabricators as well. I have attached a copy of a typical 2D drawing that we produce for this service. The clients I work for in this area all have very similar practices and have very efficient workflows that require their drawing information contained on one drawing. There are no "part" drawings and "assembly" drawings there are only "fabrication" drawings that show, sometimes several, pre- fabricated assemblies in their shipping states on the same drawing. Each item they build is custom and is unique to the type of equipment they are providing and the space it fits in. This one drawing is used for material ordering and handling, nesting, part prep, fitting, welding, document management and shipping. These drawings are used once and then discarded and this is the way they prefer the information presented.
We currently use five different (sometimes six) programs to accomplish all of the types of services we provide. Two of these are AutoDesk products. In an attempt to streamline our workflows and tools we are performing what we call a software implementation study to see if we can efficiently use IV to perform tasks we normally reserve for one of our other software platforms. Part of this study involves using the software (while others do the same project in another platform) on a project to compare, design workflows, develop project management, etc. and we are often using Inventor in ways that would be best suited for a different type of platform to test its capabilities. One of these ways is what I have described above. In this instance I need IV to give me a "parts list" for an assembly drawing that contains all of the fabrication information on that drawing for the one prefabricated assembly. There are no part drawings in this instance.
Until AutoDesk takes over the world and can provide my company with one set of tools that can handle all of my companies needs we will likely spend a lot of our own time trying to squish Inventor (or any of the other 4 programs) into a hole in which it does not fit.
Sorry about getting all "Tolstoy" on you. I appreciate the help and additional information on the iProps. The extents that I am calling in are coming in decimals of an inch though. That must one of the differences between <Sheet Metal Length> and <Flat Pattern Length>.
Have a good day!
Thanks for the lengthy explanation. Can not say I haven't heard it all before, but still appreciate you have taken your time to put it all in writing. One thing I haven't heard is that putting individual details for fabricating onto assembly drawings is required by any National Standard. It is certainly not the case in Australia. Nor in Eastern Europe.
Well, not so much "required" by the code as "adopted" by the code and made reference to in their example drawings. There is nothing specifically that states it is an exact requirement but it is the way most of the mid to small size fabricators operate. Some of the larger steel fabricators I deal with operate with part and assembly drawings (again, part of the reason we are trying to consolidate our software). My feeling is that this is something that is likely to change as technolgy changes. It is, as you are aware, technology that drives the industry and the industry that drives the codes. Thanks for the input; have a good day!
Although, not supported, the addin by Brian Ekins has been fairly robust with a few small exceptions that he has fixed when made aware.
The problem with the "Autodesk" way is that it does not handle legacy parts. The addin deals with all legacy parts as well and you do not have to add parameters etc.
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