Import Logo to Extrude

Hi..

I've been tearing some hair and firing expletives for the last 2 days trying to get what I feel should be a pretty basic requirement working in inventor 2013..

I'm looking to import a vector logo created in illustrator CS6 into inventor. I export as a dwg from illustrator which is fine but when this is inserted (or copied from autocad) All the lines are broken down into segments rather than being a continuous line from which I can extrude.. If I run sketch doctor on the imported file it complains of missing coincident constraint's even though I have the constrain end points checkbox ticked..

If you open the dwg up in autocad it seems to recognise that the lines are continuous but not in inventor.. I've read many articles some suggesting to create a true type font of the logo but this doesn;t seem to work..

can anyone tell me how this is done practically. I see that solidworks has a native adobe illustrator import and if necessary I will move to their platform as this shouldn't be as taxing as it's becoming..

thanks

This is actually not a common action to perform. In almost 9 years of professional services around Inventor involving training, implementation, and other consulting services, this is the first time I have heard this exact question. Normally companies are just fine taking the image into Inventor and using it as a label or in this case a Decal command to add vibrant logo to a design. You should also remember that Adobe doesn't own the DWG code and therefore cannot be relied on for perfect translation to Vector graphics just as Autodesk and other companies interpret PDF differently.

For what purpose do you need to extrude the logo? Is this an actual machining you are going to perform on the part? Are you 3D printing something?

Hi Mark. Thanks for your comments but this is a very common action to perform. How many times do you see a company logo embossed on a plastic part.. it's everywhere.. If I want to create a Decal I would do this in illustrator and then print it on my Roland BN-20. I want a logo embedded into the side of a plastic part as part of a mould. There are loads of article on this.. just two examples below..

http://forums.autodesk.com/t5/inventor-general-discussion/how-to-emboss-or-extrude-a-logo-or-image/td-p/5187999

http://forums.autodesk.com/t5/inventor-general-discussion/easy-way-to-do-logo-companies-with-inventor/td-p/3276161

Vector Logos are always created in corel or illustrator for use on vinyl cutters for sign writing etc.. I think Autodesk should be the ones supporting these formats not the other way around. Solidworks has been supporting illustrator files since CS3 from what I've read.. This is a pretty basic thing to support.

Having to redraw a complex vector logo in Inventor is a joke..

From the other articles I've read creating the logo as a true type font used to work. I've finally managed to get something in using this method by creating a corel draw document at 750 x 750 pts. Shrinking my logo to fit this size then exporting the document as a true type symbol font. In inventor though you have to make the size ridiculously large to even see the font (4000mm) in my case but when I try and extrude I get a self intersecting error..

This error is noted on the forums as listed above.. thus the problem remains....

How to import a logo to Inventor.. seems like the solution is to purchase solidworks.

I've probably not run into it because I've had users create their logos in Inventor or AutoCAD and the translation has been smoother but not necessarily groundbreaking art.

I would add this support option to the Inventor IdeaStation and get user response and support to add it to the software. The more Kudos it gets the more likely it is to be implemented.

Care to throw up your export DWG and I'll see if there are any other things I can process on it to make it go into Inventor in a more reliable fashion?

I understand your last statement is a vent, but believe me there are pros and cons both ways, not only in functionality but also overall software cost.

Sure here is an example of the dwg.. No designer will be producing logos in autocad but many people will want logos embossed on their products. I really cant believe autodesk has not thought of this and there doesn't even appear to be a viable work around..

qube.dwg

Okay, so you have some things going on with this export to DWG. First off, its one big block with solid fill. What I did...

I exploded the block, removed the hatch, removed the extra boundaries created by the exploded hatch. From here everything worked fine except the upper right area of the logo which had too many complex splines for Inventor to interpret in the sketcher. So I went back to AutoCAD and used SPLINEDIT with a default precision of 10 (higher would be smoother but more segments) I also ensure there were no other overlap geometry (OVERKILL is good for this, but also a manual inspection).

Truth be told if I spent an hour on this I could probably come up with a smoother profile and better geometric outputs from AutoCAD to Inventor. I also would look at my export options in the Adobe tool to see if I can get an export without splines to begin with. I would also not have the fill inside the logo either to help reduce work on this. I did my work in Inventor 2016 so I don't think I can give you the file.

I did attach the AutoCAD file that worked for me though. I also don't see this as something that would be that hard to redraw in AutoCAD if you are going to use it a lot. I could easily get rid of the facets in the upper right if I took another 20 minutes or so.

qube-poly2.dwg

Hi Mark..

Thanks I followed your suggestions and removed the hatches in autocad and converted the lines to polylines and removed the duplicates.. I now get something useable in inventor.. Still it takes an age to move or rotate.. soooo slow,,

However I can just about live with it.. One issue remains in that each part of the logo is treated separately so when I try to extrude it only extrudes the one segment that is selected..

Is there an option in AutoCAD to group these polylines so they will extrude as one?

There is tools in AutoCAD to group the data together, but that doesn't change the fact Inventor wants to select individual closed loops for profiles. I used to have a Macro that would pick them all, but you would be better off creating this as an iFeature so you wouldn't have to pick them all the time.

Thanks Mark... Tried the IFeature but same result.. I selected the sketch and then chose extract ifeature from the manage>author>extract ifeature then reimport but still only selects the individual loops rather than everything on the sketch..

wow this is complicated just to get a basic vector logo in..

ok..so I created new part an imported the dwg file. Extruded each segment individually and extruded it. saved as ipart then imported with ifeature to my part. never mind all the pre-cleanup work in autocad removing hatching and the like. It still doesn't really do what I want (needed emboss rather than extrude but cant as you can only create rather than cut in new part) but as I reached the point where I no longer want to live this will have to do.,. .. really Autodesk,, 3 days learning how to import a vector logo.? And the amount of ram to compute each move / rotate/ is insane.. auto dimension came up with something like 28,000 missing dimensions.. unless I'm missing something obvious? I'm by no means an expert..

My stp export is 28mb compare to symmetrical part using inventor sketch text (emboss) of only 2.5mb..

Well an iFeature cut would be created as first base extrusion, and then a cut and the cut can be used as an iFeature. You are right in that it should perhaps be easier to do than it is, but most advanced users can do this. I still think you should put it on the IdeaStation with a case benefit of time saved versus redrawing it in AutoCAD or Inventor, even though that is what most people do, it still would be a productivity enhancement.

Truthfully, training on this could have been done a lot quicker with a Webex or paid training support. I understand it took you a while to get where you are, but its also the reason I don't rotate my tires at my house

I would not use that geometry in Inventor - it might be OK for pretty pictures, but it is not appropriate geometry for AutoCAD or Inventor.

The geometry is so simple that I would recreate from scratch in AutoCAD or Inventor as simple lines and arcs (no splines).

It would take less than 3 hrs, let alone 3 days - and the geometry would be clean, simple geometry.