How to emboss or extrude a logo or image

[jb.zijp]

How can i emboss a logo into a part/sketch? I use inventor 2015. I managed to convert the jpg to dwg. Now i have the outlines i need. But when i want to extrude or emboss the shapes i can only select the lines and not the area's. Should i join the lines first ore something? Hope someone can help me. I searched other topics but none gave me a good answer besides tracing the lines one by one but that would take too much time and won't be as good as the original.

[JDMather]

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@jb.zijp wrote:

... I managed to convert the jpg to dwg.

 .... tracing the lines ... won't be as good as the original.

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Can you attach your dwg file here?

Sketching the image should be just as good as the original (but it is tedious).

[jb.zijp]

Thanks for the swift reply. I can not at this moment, but i can in about an
hour or four. Maybe you can make a better dwg from the attached file than
me? I use gimp or incscape, i'm not sure which one.

[JDMather]

I doubt there is any conversion software that will do a better job than you could do yourself.  There is no "Easy Button" that I am aware of (for Inventor use).

[Anonymous]

After you import the dwg into your sketch, see if the endpoints have coincident constraints.  If not, add them and then try again.

[jb.zijp]

Thanks to you both.

This what i did sofar.

Open the jpg with inkscape. Trace bitmap. Delete the original image (their on top of each other)
Safe as dxf. When saving select both Options: ROBO-Master and LWPOLYLINE
With only LWPOLYLINE selected you can't make any extrusion and with both or only ROBO-Master you can make some.
Open Inventor, start a part file, start a 2D Sketch, Insert Autocad File and select the dxf file.

Now i can extrude some parts of the logo. For the other parts i need to make seperate sketches and trace them with the Project Geometry Tool. Selecting all in once is not possible, at least when Project more than one detail in a skect i can't extrude it anymore.

So i'm a bit further but doing it this way is still tedious...making a sketch for every detail of the logo.

So i would like to know how i can prepare, repair or correct the image better so they are all correct closed lines. Tried to join or close but that won't do.

Cheers

[jb.zijp]

I just found out how the close-loop option works. I select one line of the non closed loop (why not all?) then right click to select close-loop, then wait a while...slow pc... and then select the other parts of the non-closed loop till it's closed. I have not done all the lines yet but it looks as if that's what John is saying. Is there an easier way?? 

[jb.zijp]

This is my end result, this is what i needed but i must say it took me a while. Maybe there is a quicker way round to do so, if not, please make it happen 😉

Cheers

[sam_m · Accepted solution]

I used to do this kinda thing quite easily using fonts but for some reason the last few Inventor releases (not checked 2015) have struggled with symbol fonts, which have worked with previous releases.

In the hope that Inventor gets fixed at some point and handles fonts in the same way again, here's how I (used to) work:

1) Use CorelDraw to convert the image to vector

2) strip out any background

3) combine all objects together, so it's a single shape of 1 colour

4) export as a new ttf font

5) install this font.

6) Open Inventor and create a text box in a sketch, use the font and tada, the logo appears and is easy to scale, move, rotate, etc.  (far easier than a sketch with a load of nodes and constraints.

7) You can extrude or emboss this text to provide the logo as 3d data in your model.

sadly step 7 seems to have stopped working - I'd guess about 2012 release.

Attached is the ttf font for reference:

1) right click and install

2) in any text box press "1" (without the quotes)

3) highlight this and change the font to zzz_test and tada, your logo...

I'm 90% certain this would have worked in Inventor 5 years ago but now if gives a "self interesection" error, even if you make it something massive like 200mm tall - almost as if it's trying to re-generate the symbol's profile and getting something wrong...

to remove the font:

goto Windows\Fonts and scroll to the end, find zzz_test and delete.

note.

I know this isn't a solution for you today, I'm just hoping it might be in (again) in the future and a dev might see this and realise something has changed with the way fonts are handled.

[Anonymous]

So I tried putting the .dxf in a sketch, but some of the loops came in distorted.

Opened the .dxf in Autocad, and used autoconstrain with only fixed constraints.  This takes a long time because of the complexity.

Insert the dwg into a sketch, fixed the one loop that wasn't closed.

Finish the sketch and extrude the profiles.

[jb.zijp]

Thanks, well done John!! I'll give it a try.

[Anonymous]

Hey sam_m,

I followed your instructions for exporting an image I created in Illustrator as a font. Everything went smoothly, however, does it matter under which 'font', or letter, I save it to?? I chose 'Basic Latin' and the letter 'A'. When I went to use the font in Inventor, it was completely distorted. What could I have done wrong?? Is there a system to doing this, meaning, a certain size, space within borders, etc?? This is frustrating.

Any help you could provide would be greatly appreciated! I haven't tried to use it anywhere else other than Inventor. I can provide a screenshot of the distortion, if you want. Thanks!

D

[sam_m · Accepted solution]

ok, I'm not sure with Illustrator, but here's my process with CorelDraw in the hope it helps:

1) create the shape in CorelDraw, flatten/join all parts together to give a single object of a single colour

2) create a new Coreldraw file and copy/paste into this

3) set the object to a simple size, eg 20mm

4) set the page to just fill the object - for some reason I've found this works better than just exporting the selected object.  I think it works by the bottom of the page being the baseline of the text, so anything below the bottom edge is under the text (like the tail of a g).

5) with nothing selected I goto file -> export, choose a filename and "save as type: ttf"

6) With CorelDraw I get a dialog asking for the font's name and whether it's a symbol font (yes)

7) Then the next dialog box shows the symbol and it's position on a baseline and a table to select what character the symbol should represent.  To ensure I get the same size through from CorelDraw to Inventor I change the units to the same, and the size too - here mm and 20.  Select a character (a) and then save.

😎 within Windows right-click on the ttf file and "install"

9) load Inventor, create a text box and type the letter (in this example "a"), change the font to this new one, and then the size to what you want.

10) constrain as normal and then extrude

Here's a selection of screen grabs from the various steps:

I hope that helps clarify it a little.

If it's getting distorted then could Illustrator need an update?  Or are the settings correct in its version of the "true type export" dialog (top right in image)?

If it's distorted in Character Map or Word then I guess the export is wonky.  If it's ok in Word but weird in Inventor then I guess it could be an Inventor bug?

[slv.modd]

This is in vain ; don't work.I try it 3 times.....

Another glitch is that the text from new font have a very low resolution !

The vector import tool in Inventor DON'T WORK WITH THIRD PARTY SOFTWARE ! period.

[johnsonshiue]

Hi! As I have replied to you in other threads, please attach an example exhibiting the problem. So, forum experts can comment further.

Many thanks!

[slv.modd]

I already sent you on another post the files, but I will do it again.....

Inventor import big arcs or splines, and split the arcs and splines on VERY SMALL arcs, because of this the information became huge, thousands points, but I'm sure you get the problem, my wonder is why untill years that problem remain unsolved ?

I work in woodworking, and got todo/need often to import vectors from third party/clients app vectors, unfortunate this beautiful soft (Inventor) can not solve one small problem=to let the vectors how they are native, and not to split them in very small units, another problem to solve is the sketch doctor, if someone need to repair vectors with thousands or hundred points , the command for repair let you captive (you can not leave the command untill the vectors are not solved !!! ) the only way to break the started command is to end prog from Program Manager, and of course to lose all your work.

[WHolzwarth]

That doesn't look like an Inventor problem to me.

I think, it's caused by the existing geometry in the basic DXF.

Look at the blue cloud at the f character (Screenshot from DXF)

[slv.modd]

.....this is not one answer or solved situation for importing vector tool in Inventor....

I only ask a simple question :

Why the big arcs or splines are splitted on very small arcs or splines after vector are imported in Inventor ?

Is anybody able to answer or not !?

[WHolzwarth]

It's the GIGO syndrom: Garbage in - Garbage out.

I've looked at your second file in the other thread, too. It's even worse, because all geometry has triple outlines.

The fonts are made of splines with lots of control points. These are imported one by one into Inventor.

[-niels-]

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@slv.modd wrote:
...

I work in woodworking, and got todo/need often to import vectors from third party/clients app vectors...

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@slv.modd, i'm not familiar with the software myself, but i've seen @kelly.young promote Artcam a lot for this kind of thing.

Check it out here:

https://www.autodesk.com/products/artcam/overview

Might be what you're looking for.