Autodesk Wiki Help says this: "Decals may be stocked and have part numbers. If this is a requirement, consider creating the decal in its own part file. You can then insert it into an assembly and use assembly constraints to position it." Now this is possible but you can not wrap or face the decal in the assembly mode, let say on a piece of pipe. The only way to wrap of face is modifying a part, adding the decal, but then you don't get a part number in a BOM because its not a separate part. Does anyone have a solution?
Hi aaron.seifert,
I prefer to handle this with an iPart factory. Attached is a simple example. The wrap diameter is set when placing the part into an assembly.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hi Curtis,
I realise this is an old(ish) post but I have used your method to create a label (in an ipart) however when I add it into the assembly the graphics don't actually show the label. Is there any way to get this to show?
Thanks,
Chris
Hi CNewman,
My apologies for the misinformation.
My focus when creating this post must have been on the changing of the diameter and getting the part number in the BOM, more so than the image.
The image will not show in the iPart member files as you've noticed, because iParts are essentially derived parts, and the derived part tools do not support image decals.
Honestly, I use a variety of workarounds to get the results we need for this when showing an image is needed, but I doubt any of them are too practical. For the most part we use this iPart approach for numbered labels where the text and logo are extruded features, and it works well. Even when we use an image decal, our focus is on getting the correct part number of the label in the BOM.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Thanks Curtis,
I half expected as much as there seems to be a fair bit you cannot show/use when using iParts. I'm pretty new to Inventor (as a seasoned ProEngineer user) so it's all a bit of a learning curve for me at the moment but we're getting there.
Appreciate your help though.
Regards, Chris
instead of using iParts could you get the same result by using the export (and linked) parameters?
presumably the parent pipe's diameter is a value in its parameter table, if so then set it to export.
for the decal, create a new file and goto the parameter table and "link" pointing to the parent ipt and select the exported value (has a v small green arrow over the x in the collumn). Use this as the inner diameter of a curved label and extrude the label's dimensions and decal the image wrapped to that.
now have 2 parts (for the BOM) linked without iparts. Or have I missed something?
Sam M.
Inventor and Showcase monkey
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Thanks for your suggestion, i'll have to have a play with this and see if I can't find something that will work for us.
I thought that you could only place a decal on a part, not assembly? How can you place it into an assembly?
@Anonymous wrote:I thought that you could only place a decal on a part, not assembly? How can you place it into an assembly?
You can simply create a new part...extrude a surface the same size as the decal, attach a decal image to it and save that as a part..then place that part into any assembly.
I am not sure I follow you. In the assemblies I am refering to are stencils that need to show up in the drawing for electrical designations. If I make an extruded surface and create a new part, I am not sure how I can get that to show
in the assembly.
Lets try this again.. You said you could only apply a decal to a part.. Which is correct. Then you simply insert that part into an assembly just like any other part.
Basically doing an extruded surface and applying the decal to that is a simple way to basically make a "sticker" part that can then be inserted into any assembly and constrained just like any other "regular" part.
The extruded surface is simply the "paper" of the sticker and the decal is the image printed on that paper.
By "stencil" I assume you are talking about a "silk screened" type marking that is applied to something. If so... I find its best to simply create the text/shapes and then extrude them (.001" thick or so) in a part file.. Then insert that part into the assembly. The big benefit of that is that when you do the drawing a "decal" requires a shaded view to even see the image (stupid move autodesk IMO) where extruded text will show up in any type of view (shaded/hidden lines,etc..) as long as you don't mind a "double" line font because it will show the outlines of the text in the drawing.. But to me that is FAR better than having to do shaded views..
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