Hi, new to Inventor and its properties. I would like to define a Sketch Symbols Standard Note in my sheet metal drawing with the following headings-
FILE NAME: easy to insert
MATERIAL: easy to insert
THICKNESS: ? - would like to see "3mm" as it is the part thickness
FINISH: ? - would like to see "-2B" as this is the finish as specified in the part
QTY: ? - promoted for a value
SCALE: ? - flat pattern scale
I have defined custom iProperties for the THICKNESS and FINISH in the part file but it doesn't bring it across to the drawing. I would like to have a promoted input for QTY. The SCALE is to ensure the flat pattern is at scale 1:1.
Some help would be appreciated please.
Solved! Go to Solution.
Solved by jtylerbc. Go to Solution.
Some of what you are asking for is extremely simple. Others not so much. I'll start you off with some help on the easier portions.
@john.vanderhoven wrote:
THICKNESS: ? - would like to see "3mm" as it is the part thickness
FINISH: ? - would like to see "-2B" as this is the finish as specified in the part
If you have already created custom iProperties for these items, then inserting them into a symbol is no different from any of the properties you have already figured out, except for one critical point. You must place a view in the drawing of a part that contains the properties. Once you have done that, those properties will show up under "Custom Properties - Model" category. Until you place the view, this entire category is omitted from the dropdown list.
Once you create the symbol, it can be copy-pasted into any drawing, and the properties will just show up as blank if they don't exist. But to create them initially, you must have a view placed from a part that contains them. Inventor has no idea those properties exist until you do so.
@john.vanderhoven wrote:
QTY: ? - promoted for a value
SCALE: ? - flat pattern scale
These items are more difficult. With more information about your specific application, it may be possible to solve them as well, but the solution will probably involve custom programming. There are specific reasons why this is the case. Not knowing the details of your application, I'll explain why these items are issues instead of proposing specific solutions at this point.
Depending on the specifics of your usage, there may be ways around this. For example, let's say your parts are always specific to a particular assembly, and never get reused (common in welded structures, for example). It might be possible to write some iLogic code in the assembly that reads the part quantity and writes it to a custom property in the part. You can probably search these forums a bit and find discussions about this topic, possibly even with sample code.
Similarly, if your drawing only contains one view, it might be possible to write code that reads that scale and writes it to a custom property of the drawing, which could then be used in the symbol. If the drawing contains multiple views but only one flat pattern view, it might still be possible to write the code in such a way that it ignores all the views except the flat pattern.
Regarding the Scale, if the only reason to have it is to check that it is 1:1, another option might be to write code that simply forces all views in that drawing to be 1:1 scale when the drawing is saved. This may arguably be better, since instead of just giving a method to check for the problem, it directly fixes it.
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