Extruding Line Drawings from Adobe Illustrator

[18922014]

Hey Everyone,

I am having some trouble trying to create a thin line extrusion in Inventor from drawings created in Adobe Illustrator. The drawings were originally .eps vector files from Illustrator, and I've been able to export the files from Illustrator as .dwg, import into Autocad and copy/paste the drawing into Inventor, but after this I'm stumped. Is Inventor even capable of doing single line extrusions, or does it absoutely need to be a closed profile?

Ideally I am trying to raise the line segments about half a mm, while widening or thickening the stroke width of the lines to about 1mm. Then print these onto a thin plate so individuals can feel the raised lines with their fingers. I've made some moderate progress using Solidworks' thin line extrusion, but I am not as familiar with SW as I am with inventor.

I've attached the exported .dwg and the part file I created after using Autocad.

Let me know what you all think would be the best approach to this, any information would be greatly appreciated!

Thanks,

Landon.

[mcgyvr]

Inventor can do single line extrusions.. BUT they are just a surface at that point.

I didn't open your files but I suspect the "constrain end points" setting when inserting the autocad file is what you want to do.. That will automatically apply constraints to all the intersections thus turning them into closed profiles.

see attached..

I start a new sketch then hit the insert "ACAD" button and pick the dwg file then a dialog opens.. hit the next button and you will find this screen

[18922014]

Thanks for the response, mcgyvr.

Using that method to import the dwg did cut out the need to first open and copy it from autocad, but I am still left at the same point I was at before. I cannot figure out a way to raise the lines themselves, instead it is trying to extrude only the closed sections. I see that I can do a surface extrusion, but then I am unsure of how to create the proper width of the extruded lines.

If you get the chance, take a look at the dwg I attached in the original post. The object is fairly simple, it just seems like trying to figure out how to do this extrusion with the proper width is a bit more complex than I anticipated.

-Landon

[mpatchus]

You could offset the lines to the desired thickness, then extrude the "outline" to the desired height.

See attached.  

(Really quickly done without constraints just to illustrate the process.)

[JDMather]

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@18922014 wrote:
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 but then I am unsure of how to create the proper width of the extruded lines.

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Use the Thicken command.

[mcgyvr]

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@18922014 wrote:

Thanks for the response, mcgyvr.

Using that method to import the dwg did cut out the need to first open and copy it from autocad, but I am still left at the same point I was at before. I cannot figure out a way to raise the lines themselves, instead it is trying to extrude only the closed sections. I see that I can do a surface extrusion, but then I am unsure of how to create the proper width of the extruded lines.

If you get the chance, take a look at the dwg I attached in the original post. The object is fairly simple, it just seems like trying to figure out how to do this extrusion with the proper width is a bit more complex than I anticipated.

-Landon

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Sorry.. I didn't read all of your original post..

But looks like mike and jd already answered that for you..

[18922014]

Sorry for the delay, been a busy week and I'm just now getting back to trying to solve this design. I appreciate the help! So far I've gotten the .eps drawing imported in autodesk, the proper thickness and height extruded properly, but I have some gaps and uneven secitons in the feature that I am having a bit of trouble getting to fit together correctly. Take a look at the attached wine glass file and you will see what I mean. I did several surface extrusions and then thickened them to the proper thickness. Does this seem like a feasible way of doing this, or is there another more straightforward approach?

I also want to round out the upper edges on the feature to have a uniform curve to them rather than the sharp edges. Is there an easy way to go about this other than trying to fillet each edge? Ideally the curve would match the curve of the dot shape I've attached.

Thanks again for the help...I am still getting a grasp with this software and any help is appreciated.

-Landon

[JDMather]

If the geometry is generally that simple - I think I would just trace overtop in a new sketch.

I suspect Swept features might be what you are after.

This was even easier than I thought it would be.

Now I would Sweep some circles and then Spilt or extrude off the bottom to make flat.

I had to do this realllll fast and didn't get it exactly the way I wanted.

(see attached file)

[JDMather]

Is something like this what you are after?

[18922014]

JDMather, those look fantastic! I would say thats about 99% what I'm looking for, and I'm sure I can figure out the last little bit.

I've tried tracing over the images in the past, but never had much luck. Would you mind explaining a bit more about the steps you took to get there? Again, I'm still getting a grasp on Inventor and I haven't practiced with swept features all that much. I see you performed several sweeps, but how did you get the flat surface on the bottom, was that from the final split operation?

Thanks again for your help, I really appreciate the time you've put towards this so far!

-Landon

[JDMather]

I'll come back later with more of an explanation when I have time, but -

You can reverse-engineer how something was done in Inventor by dragging the red End of Part marker to the top of the browser and then back down step-by-step.

[JDMather]

Did you figure this out?

[18922014]

For the most part I understand what you did with the wine glass. I am having a bit of trouble applying it to some of the other, more complex drawings I have. Is there any way to use the imported dwg images and create the proper swept features other than simply resketching the entire line drawing first? I attempted using the same tools/actions you performed with the wine glass on another drawing, and basically got hung up trying to complete the new traced sketch.

I also was hoping you could clarify how you performed the final split function. From what I can tell, you created an offset plane at the proper height so that the remaining feature would be 0.43mm high, then split or cut away all of the material below this plane. Is this correct?

[JDMather]

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@18922014 wrote:
 From what I can tell, you created an offset plane at the proper height so that the remaining feature would be 0.43mm high, then split or cut away all of the material below this plane. Is this correct?

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That is what I did.

As far as using the dwg geometry without tracing - that works fine as long as the geometry is good quality.

In my experience, geometry coming from Illustrator is not good quality for use in Inventor.