Quick backstory: I set up our company log which gets embossed on most parts as a sketch block in an .ipt. The .ipt contains nothing but the sketch block. To use it, the designer only needs to derive the Logo.ipt file into their part and then use the scale setting to set the derived block to the desired size for that part. The result is a scalable set of line geometry that can easily be used for extrusion or emboss that is standard for all users. It works beautifully, that is until you try to use it in a sheet metal part in 2012.
For some reason, when this same part, which works perfectly in normal parts, is derived into a sheet metal part an error pops up stating that, "Selected part does not have any geometry that can be derived." Say what?
I was able to find a workaround by directly copying the block into the sheet metal part, but you no longer have the ability to go back and scale it if needed. Even more strange, when the block was copied over, it could not be deleted from the new part.
Is this just a bug with 2012? Why does it work in a normal part but not sheet metal?
Sheet metal parts are different then a normal ipt or machined part. This maybe part of the reason your experiencing this issue. Did it work in Inventor 2011? If so I would like to look at a sample file and the block in quesiton. If it didn't then it may be the nature of the part file.
@mercerc, I thought it worked in 2011, but am not certain. It's rare that it's used with sheet metal parts, typically only when something needs to be laser etched, but that's done better with line artwork.
Either way, there is no justifiable reason why this shouldn't work in sheet metal other than it's a bug or an oversite. I can send you the specific file I'm using, but it's not necessary. You can recreate the issue very easily. I tried a test version from scratch and had the same issue, so this is not part specific.
I've attached a sample part. Try to derive that into a sheetmetal part to see what I'm talking about.
This is a inconsistant workflow issue with Inventor that needs to be fixed.
Sorry to tack this onto this discussion, but the forums wouldn't let me send pberry a private mesage (apparently there are three pberry accounts).
A side question regarding your post on deriving a logo "master" part into parts for embossing, etc. I like your method since it gives control over the logo size and consistency since many parts can be derived from one "master" logo.
However, when deriving the part, how do you control its location. E.g. if I want the logo to go in the top left corner, how do I achieve that? When I derive the logo, its location is determined by the part origin and the logo part origin.
Thanks Matthew. I use a block of the sketch geometry rather than just the sketch precisely for that reason. When you derive in the block, all it does is place the block in the new part's blocks folder. From there you can place it and position it in any sketch. From there its just a matter of using extrude or emboss to turn it into geometry. It's not a perfect solution but it works pretty good.
I came up with this method after we changed our corporate logo. With the old logo someone had long ago created a windows font that contained it. All you had to do was enter 1 in the company font and you got the standard logo. This worked great in Inventor since all you had to do was add this one piece of text in a sketch and then emboss or extrude would grab the whole logo. The downside is that every PC in the company had to have this font file installed on it which became a pain for IS.
As a result when they did the redesign I had a very generous person in this discussion group make a new font for me (thanks again for that!) which worked great, but I wasn't allowed to use it. That's when I came up with deriving in blocks. It's the only way I've found in Inventor to get the spline based line geometry to scale uniformly.
That is downright awesome. My only issue is that we have text in our logo and it doesn't play well with sketch blocks. I think I'll try creating geomtry using my sketch and then create a second sketch for creating the sketch block that uses projected geometry.
I got this to work in 2012. While I have other things going on with my logo, I think what worked was to create solid geometry (e.g. simpe extrude), then completely remove it with an extruded cut (make sure to turn off visibility for all sketches so they don't get pulled in by default during the derive process). I think this provides inventor with "geometry that can be derived" that it seems to need for sheetmetal parts.
I derived my logo into a sheetmetal part and it worked.
Thanks for the workaround. That gives me some options for when this comes up again in the future.
It still bugs me that unnecessary features have to be left in the part which is why I still consider this a bug that needs to be fixed. One of those key aspects of product usability that Autodesk has been working on for the last 5 years is workflow consistancy. They've made big strides but aren't quite there yet.
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