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Thread: syntax with iproperties

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    Default syntax with iproperties

    Hello everyone. I'm new to the forum and fairly new to inventor. I'm detailing steel parts for large tanks that is done in a structural steel shop. I've figured out there is a linking ability with the parts to the bill of materials(BOM). So far I have found that I can link some of the iproperties to the bill of materials and I just found out about the custom tab, which I think is going to be a big help. I have used the custom tab to link a few things.

    I want to make this as automated as possible so I am doing little work manually with the BOM. One thing I am wondering is if there is syntax that can be written to calculate the length in the parts Iproperties, so if I were to change the part it would automatically change in the BOM in an assembly drawing. I'm not sure how I need to go about this or if its possible.

    If you have questions on what I'm trying to explain please let me know. I'm having a hard time explaining. Any help is appreciated.

    Thanks

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    100 Club Paul Munford's Avatar
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    Default Re: syntax with iproperties

    First, you need a parameter called 'Length' that is hooked up to the length of your part. Then you need to set this parameter to 'Export' to make sure it shows up in your parts custom iProperties. Next you need to add a custom iProperty column to your BOM to read out the part. Finally you will need to edit your parts list style if you want to length of the parts to show up in the drawing.

    Let me know if you have any specific questions about the process!

    -Paul-

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    Default Re: syntax with iproperties

    First, you need a parameter called 'Length' that is hooked up to the length of your part. Then you need to set this parameter to 'Export' to make sure it shows up in your parts custom iProperties.
    Can you explain how you do this?

    Thanks

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    Default Re: syntax with iproperties

    1. Open the parameters manager (the button with Fx on it)
    2. Create a new parameter and call it 'Length'.
    3. Check the box next to it marked export

    The Length parameter will define the length of your part. You can create parameters for width and thickness as well if you need to.

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    Default Re: syntax with iproperties

    Thanks for the help. For the most part I think I figured it out after fallowing your steps and a bit of trial and error.

    When I tried to create a length in the parameters I made the equation column equal to one or two of the other parameters. With a bent plate I had to do an equation of something like =d4+d12 in order to get the right length. Am I doing it this right way or is there a better way to go about it. Does it matter if you are in a flattened view or not for a bent piece of material?

    One thing I had trouble with was trying to manipulate the part mark numbers. I think it places a mark number associated to the order you placed them into your assembly. If I want to make them specialized to my own marking system how would I go about it? I tried to create a custom name with the same BOM column name but it didn't work.

    Thanks again I really appreciate the help.
    Last edited by chris.sones827586; 2012-04-17 at 09:12 PM.

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    Default Re: syntax with iproperties

    Could this be done in the sheet metal environment? The sheet metal environment has it's own tools for getting the unfolded length, width and thickness from a part:
    http://usa.autodesk.com/adsk/servlet...linkID=9242018
    http://www.microconcepts.co.uk/membe...eNum=0&blk=178

    Item numbers can be Alpha or numeric only, but you can pull your own part numbers through if you want:
    http://wikihelp.autodesk.com/Invento...32-Manage_i532

    Read 'Creating a custom Item Number Balloon' about half way down this page for an explanation.
    http://cadsetterout.com/inventor-tut...ge-assemblies/

    Keep up the good work!

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    Default Re: syntax with iproperties

    It is nice they have the =<plate pattern xxx> option to do the calculating for you, but it only works in cm as far as the articles say. I could easily change this if divided by 2.54 to get inches. Then I could format the column to ft which would work....How do I get the equation to work with the =<plate pattern xxx> ( this doesn't work but here is an example: =<(plate pattern length/2.54>)? I've tried to use different methods but can't seem to come up with anything that will work. I'm not sure if I need to do something in the functions or the custom property. So far I think the only place that the =<plate pattern xxx> works is in the iproperties in the customs tab.

    I haven't had a chance to mess with the mark numbers yet. I'm hoping to figure the majority of this out so I can have a meeting with another employee and supervisor. Once we go over some of this and see how we can implement it, I'm hoping we can come up with a better template and start modifying standard parts.

    Thanks
    Last edited by chris.sones827586; 2012-04-18 at 09:54 PM.

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    Default Re: syntax with iproperties

    I don't think that you can change the units within the formula. However you can convert the units when you place the parts list on the drawing:
    Check out this one again:
    http://www.microconcepts.co.uk/membe...eNum=0&blk=178

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    Default Re: syntax with iproperties

    I believe I played with the parts list properties the other week trying to convert this. This is the problem I remember running into. You can make the units that are transferring from the function/custom properties to the parts list change to feet and inches, but the inventor function/equation (=<plate pattern xxx>) only provides units in cm (lets say 54cm). The parts list will see 54 as units and convert it to 54 inches, which isn't the correct measurement. It needs to be converted/divided by 2.54 to get inches.

    Hope that makes sense.

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    Default Re: syntax with iproperties

    Hi Chris,

    It's important that your formula includes the Units, so that Inventor knows what units it is converting to and from.
    i.e:
    =<FLAT PATTERN LENGTH> cm

    You don't have to show the units string in the parts list if you don't want to...

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