I am doing a project now for a customer that wants his logo embossed on the
part.  He gave me with a .pdf file of his logo.   It is basically very fancy
text with lots of loopity-loops and such.  I need to get this logo into a
sketch so that I can extrude it.

I first tried to save it as a graphics image and use WinTopo to create the
geometry.  This failed.  The geometry wasn't even close to being usable.

I then called the graphics designer directly.  She uses Adobe Illustrator.
She told me that she could export it as a .dxf or .dwg though she had never
done this before.

The first attempt produced nothing but crosshatch when opened in AutoCAD,
and absolutely nothing when imported into SolidWorks.

She found some export settings or something and re-exported.

This time it opened perfect in AutoCAD, but only about 50% of the entities
(splines) would import into SW.  I got this error message:
Entity not imported, type Spline, Handle: 8C
Entity not imported, type Spline, Handle: 86
Entity not imported, type Spline, Handle: 7F
Entity not imported, type Spline, Handle: 79
etc.
etc.

I know nothing about Adobe Illustrator.  And she knows nothing about
exporting it to CAD.  Does anyone know of a way that I could get this done?
I am all out of ideas.

TIA
-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)

This is what I'd try.
Open in autocrap, select all and explode
keep doing this until there's nothing left to explode.
Save, open back up then purge all then save , close
open back up, purge all, save ,close
Keep doing this until there's nothing left to purge.
Export as dxf then try to import into SW SLDDRW.
If that works then try to copy /paste into sketch
Not sure if It'd work. but that's what I'd try
Cheers
Frank

Seth Renigar wrote:

> I am doing a project now for a customer that wants his logo embossed on the
> part.  He gave me with a .pdf file of his logo.   It is basically very fancy
> text with lots of loopity-loops and such.  I need to get this logo into a
> sketch so that I can extrude it.
> 
> I first tried to save it as a graphics image and use WinTopo to create the
> geometry.  This failed.  The geometry wasn't even close to being usable.
> 
> I then called the graphics designer directly.  She uses Adobe Illustrator.
> She told me that she could export it as a .dxf or .dwg though she had never
> done this before.
> 
> The first attempt produced nothing but crosshatch when opened in AutoCAD,
> and absolutely nothing when imported into SolidWorks.
> 
> She found some export settings or something and re-exported.
> 
> This time it opened perfect in AutoCAD, but only about 50% of the entities
> (splines) would import into SW.  I got this error message:
> Entity not imported, type Spline, Handle: 8C
> Entity not imported, type Spline, Handle: 86
> Entity not imported, type Spline, Handle: 7F
> Entity not imported, type Spline, Handle: 79
> etc.
> etc.
> 
> I know nothing about Adobe Illustrator.  And she knows nothing about
> exporting it to CAD.  Does anyone know of a way that I could get this done?
> I am all out of ideas.
> 
> TIA

Frank,

I had interesting results doing this.

Before, there were 17 splines that wouldn't import which made up approx.
70-80% of the geometry.  So I only got around 20-30% actual good geometry.

After exploding as you suggested, there were 72 splines that didn't import.
But since there was a LOT more splines to start with, that still left about
80-90% of the geometry that DID import.  I think I may be able to fudge the
last 10-20% by tracing over a sketch picture.

To trace the whole image would have taken days.  This at least reduces that
time to a somewhat tolerable level.

Thanks for the suggestion.  I'll have to remember that...

-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)


"FrankW" <fworm@mxznorpak.ca> wrote in message
news:K8qdnTuwuPj2wujcRVn-pQ@magma.ca...
> This is what I'd try.
> Open in autocrap, select all and explode
> keep doing this until there's nothing left to explode.
> Save, open back up then purge all then save , close
> open back up, purge all, save ,close
> Keep doing this until there's nothing left to purge.
> Export as dxf then try to import into SW SLDDRW.
> If that works then try to copy /paste into sketch
> Not sure if It'd work. but that's what I'd try
> Cheers
> Frank
>
> Seth Renigar wrote:
>
> > I am doing a project now for a customer that wants his logo embossed on
the
> > part.  He gave me with a .pdf file of his logo.   It is basically very
fancy
> > text with lots of loopity-loops and such.  I need to get this logo into
a
> > sketch so that I can extrude it.
> >
> > I first tried to save it as a graphics image and use WinTopo to create
the
> > geometry.  This failed.  The geometry wasn't even close to being usable.
> >
> > I then called the graphics designer directly.  She uses Adobe
Illustrator.
> > She told me that she could export it as a .dxf or .dwg though she had
never
> > done this before.
> >
> > The first attempt produced nothing but crosshatch when opened in
AutoCAD,
> > and absolutely nothing when imported into SolidWorks.
> >
> > She found some export settings or something and re-exported.
> >
> > This time it opened perfect in AutoCAD, but only about 50% of the
entities
> > (splines) would import into SW.  I got this error message:
> > Entity not imported, type Spline, Handle: 8C
> > Entity not imported, type Spline, Handle: 86
> > Entity not imported, type Spline, Handle: 7F
> > Entity not imported, type Spline, Handle: 79
> > etc.
> > etc.
> >
> > I know nothing about Adobe Illustrator.  And she knows nothing about
> > exporting it to CAD.  Does anyone know of a way that I could get this
done?
> > I am all out of ideas.
> >
> > TIA
>

You might try saving to an older version of dxf that doesn't support spline 
entities. You may need to use the dwgEditor to do this. IIRC, R10 or 11 
should do. The spline should then be saved as lines and arcs.

I could easily be completely worng though. That was a long time ago.

That does work.  I saved it as R12 dxf.  But there were so many lines that
it brought SW to its knees.

I tried to window select all of the lines in the sketch.  I sat there and
waited about 4-5 minutes as all of the lines turned green one by one.  I did
get a pop-up message that I had never seen before in the 8 years I have been
using SW.  It said: "Not all of the large number of entries can be listed".
I figure there must have been many thousand lines in the sketch.

This would probably work great on smaller geometry.  Oh well.  Back to the
"drawing" board...

-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)


"Dale Dunn" <daledunnSCRATCH@jamestool.com> wrote in message
news:Xns9587A35C59B63daledunnatjamestoolc@65.24.7.50...
> You might try saving to an older version of dxf that doesn't support
spline
> entities. You may need to use the dwgEditor to do this. IIRC, R10 or 11
> should do. The spline should then be saved as lines and arcs.
>
> I could easily be completely worng though. That was a long time ago.

Any chance of extruding it in ACAD and exporting the bodies into SW via 
ACIS?

Here's the trick to make it work Seth.  Open the version 12 drawing in
AutoCAD.  Once open type PEDIT at  the command line.  Type "M" ENTER to
select multiple entities.  Window select the entire drawing.  When asked to
convert to poly lines say YES and Enter.  Next Hit "J" and ENTER to join all
the lines.  Input a "fuzz distance".  I usually use .06 but you may need
something different.  Hit Enter and let it do it's thing.  When done save
the drawing.  What you just did was turn everything in to poly lines, closed
99% of the gaps and connected all the poly lines together.

Now open this drawing into a part file in SW.  When doing this set the merge
points option to a low number like .01.  It should open with out problems
and you should have closed contours for extruding.  If not you can use the
sketch tools to show you where the holes are.  There should only be a couple
if any.  I regularly do this with dwg files that have thousands of line
entities with no problems.  Let me know if you need more help.

Rob





"Seth Renigar" <SpamFree_srenigar@SpamFree_emeraldtoolandmold.com> wrote in
message news:T0ddd.27740$zA3.4400969@twister.southeast.rr.com...
> I am doing a project now for a customer that wants his logo embossed on
the
> part.  He gave me with a .pdf file of his logo.   It is basically very
fancy
> text with lots of loopity-loops and such.  I need to get this logo into a
> sketch so that I can extrude it.
>
> I first tried to save it as a graphics image and use WinTopo to create the
> geometry.  This failed.  The geometry wasn't even close to being usable.
>
> I then called the graphics designer directly.  She uses Adobe Illustrator.
> She told me that she could export it as a .dxf or .dwg though she had
never
> done this before.
>
> The first attempt produced nothing but crosshatch when opened in AutoCAD,
> and absolutely nothing when imported into SolidWorks.
>
> She found some export settings or something and re-exported.
>
> This time it opened perfect in AutoCAD, but only about 50% of the entities
> (splines) would import into SW.  I got this error message:
> Entity not imported, type Spline, Handle: 8C
> Entity not imported, type Spline, Handle: 86
> Entity not imported, type Spline, Handle: 7F
> Entity not imported, type Spline, Handle: 79
> etc.
> etc.
>
> I know nothing about Adobe Illustrator.  And she knows nothing about
> exporting it to CAD.  Does anyone know of a way that I could get this
done?
> I am all out of ideas.
>
> TIA
> -- 
> Seth Renigar
> Emerald Tool and Mold Inc.
> (Remove "SpamFree_" from my address)
>
>
>

I did try this.  It processed for around 40 minutes and never finished.  I
needed my machine back so I had to end the task before completing.  I will
try this again today just before I leave work so that I can let it process.

By the way, I assume the "fuzz distance" of .06 is metric.  I entered .002
for inches (should be about the same).

FYI - There are about 58000 lines in this logo drawing after exploding
everything.

-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)


"Rob Rodriguez" <toyrock@pshift.com> wrote in message
news:Cyhdd.827$bz.326@fe39.usenetserver.com...
> Here's the trick to make it work Seth.  Open the version 12 drawing in
> AutoCAD.  Once open type PEDIT at  the command line.  Type "M" ENTER to
> select multiple entities.  Window select the entire drawing.  When asked
to
> convert to poly lines say YES and Enter.  Next Hit "J" and ENTER to join
all
> the lines.  Input a "fuzz distance".  I usually use .06 but you may need
> something different.  Hit Enter and let it do it's thing.  When done save
> the drawing.  What you just did was turn everything in to poly lines,
closed
> 99% of the gaps and connected all the poly lines together.
>
> Now open this drawing into a part file in SW.  When doing this set the
merge
> points option to a low number like .01.  It should open with out problems
> and you should have closed contours for extruding.  If not you can use the
> sketch tools to show you where the holes are.  There should only be a
couple
> if any.  I regularly do this with dwg files that have thousands of line
> entities with no problems.  Let me know if you need more help.
>
> Rob
>
>
>
>
>
> "Seth Renigar" <SpamFree_srenigar@SpamFree_emeraldtoolandmold.com> wrote
in
> message news:T0ddd.27740$zA3.4400969@twister.southeast.rr.com...
> > I am doing a project now for a customer that wants his logo embossed on
> the
> > part.  He gave me with a .pdf file of his logo.   It is basically very
> fancy
> > text with lots of loopity-loops and such.  I need to get this logo into
a
> > sketch so that I can extrude it.
> >
> > I first tried to save it as a graphics image and use WinTopo to create
the
> > geometry.  This failed.  The geometry wasn't even close to being usable.
> >
> > I then called the graphics designer directly.  She uses Adobe
Illustrator.
> > She told me that she could export it as a .dxf or .dwg though she had
> never
> > done this before.
> >
> > The first attempt produced nothing but crosshatch when opened in
AutoCAD,
> > and absolutely nothing when imported into SolidWorks.
> >
> > She found some export settings or something and re-exported.
> >
> > This time it opened perfect in AutoCAD, but only about 50% of the
entities
> > (splines) would import into SW.  I got this error message:
> > Entity not imported, type Spline, Handle: 8C
> > Entity not imported, type Spline, Handle: 86
> > Entity not imported, type Spline, Handle: 7F
> > Entity not imported, type Spline, Handle: 79
> > etc.
> > etc.
> >
> > I know nothing about Adobe Illustrator.  And she knows nothing about
> > exporting it to CAD.  Does anyone know of a way that I could get this
> done?
> > I am all out of ideas.
> >
> > TIA
> > -- 
> > Seth Renigar
> > Emerald Tool and Mold Inc.
> > (Remove "SpamFree_" from my address)
> >
> >
> >
>
>
>

Seth,

Download a demo of rhino and use it's arcfit command (under edit menu - I 
forget exactly what it's called) it will 'trace' the splined version of your 
dxf with a series of tangent arcs.  Or just use rhino to extrude/model 
whatever 3d features you want for the logo and import these into sw to use 
as toolbodies.

Or as Dale suggested - extrude the closed shapes in autocad to primitive 
solids then import these into solidworks,  you can use these solids as 
toolbodies or just create sketches from the faces.

Save out the logo as a tif or bitmap and use a raster to vector program 
(flexisign has a good one) to convert in 100% closed splines.  (Helps 
simplify the geometry without losing the shape, also works great for clipart 
which is always got overlapping sections)

Also,  a vastly overlooked autocad tool:  part of the express tools is 
called 'overkill' at the command line,  I think the menu item is called 
'find duplicates' or something,  it is similiar to multi pedit but does a 
lot more and works very well.

Also,  if you have access to mdt (mechanical desktop) it has a spline to 
pline command on the surfacing toolbar.

Zander


"Seth Renigar" <SpamFree_srenigar@SpamFree_emeraldtoolandmold.com> wrote in 
message news:oJsdd.30980$n%3.4298373@twister.southeast.rr.com...
>I did try this.  It processed for around 40 minutes and never finished.  I
> needed my machine back so I had to end the task before completing.  I will
> try this again today just before I leave work so that I can let it 
> process.
>
> By the way, I assume the "fuzz distance" of .06 is metric.  I entered .002
> for inches (should be about the same).
>
> FYI - There are about 58000 lines in this logo drawing after exploding
> everything.
>
> -- 
> Seth Renigar
> Emerald Tool and Mold Inc.
> (Remove "SpamFree_" from my address)
>
>
> "Rob Rodriguez" <toyrock@pshift.com> wrote in message
> news:Cyhdd.827$bz.326@fe39.usenetserver.com...
>> Here's the trick to make it work Seth.  Open the version 12 drawing in
>> AutoCAD.  Once open type PEDIT at  the command line.  Type "M" ENTER to
>> select multiple entities.  Window select the entire drawing.  When asked
> to
>> convert to poly lines say YES and Enter.  Next Hit "J" and ENTER to join
> all
>> the lines.  Input a "fuzz distance".  I usually use .06 but you may need
>> something different.  Hit Enter and let it do it's thing.  When done save
>> the drawing.  What you just did was turn everything in to poly lines,
> closed
>> 99% of the gaps and connected all the poly lines together.
>>
>> Now open this drawing into a part file in SW.  When doing this set the
> merge
>> points option to a low number like .01.  It should open with out problems
>> and you should have closed contours for extruding.  If not you can use 
>> the
>> sketch tools to show you where the holes are.  There should only be a
> couple
>> if any.  I regularly do this with dwg files that have thousands of line
>> entities with no problems.  Let me know if you need more help.
>>
>> Rob
>>
>>
>>
>>
>>
>> "Seth Renigar" <SpamFree_srenigar@SpamFree_emeraldtoolandmold.com> wrote
> in
>> message news:T0ddd.27740$zA3.4400969@twister.southeast.rr.com...
>> > I am doing a project now for a customer that wants his logo embossed on
>> the
>> > part.  He gave me with a .pdf file of his logo.   It is basically very
>> fancy
>> > text with lots of loopity-loops and such.  I need to get this logo into
> a
>> > sketch so that I can extrude it.
>> >
>> > I first tried to save it as a graphics image and use WinTopo to create
> the
>> > geometry.  This failed.  The geometry wasn't even close to being 
>> > usable.
>> >
>> > I then called the graphics designer directly.  She uses Adobe
> Illustrator.
>> > She told me that she could export it as a .dxf or .dwg though she had
>> never
>> > done this before.
>> >
>> > The first attempt produced nothing but crosshatch when opened in
> AutoCAD,
>> > and absolutely nothing when imported into SolidWorks.
>> >
>> > She found some export settings or something and re-exported.
>> >
>> > This time it opened perfect in AutoCAD, but only about 50% of the
> entities
>> > (splines) would import into SW.  I got this error message:
>> > Entity not imported, type Spline, Handle: 8C
>> > Entity not imported, type Spline, Handle: 86
>> > Entity not imported, type Spline, Handle: 7F
>> > Entity not imported, type Spline, Handle: 79
>> > etc.
>> > etc.
>> >
>> > I know nothing about Adobe Illustrator.  And she knows nothing about
>> > exporting it to CAD.  Does anyone know of a way that I could get this
>> done?
>> > I am all out of ideas.
>> >
>> > TIA
>> > -- 
>> > Seth Renigar
>> > Emerald Tool and Mold Inc.
>> > (Remove "SpamFree_" from my address)
>> >
>> >
>> >
>>
>>
>>
>
> 

As my I.D. days get further and further behind me, it gets harder to
remember these things.

If you have access to Adobe Illustrator, then you may be able to do
some editing to prepare for the export.  Crosshatches?  There is no
need for filled blocks.  Create outlines and remove block shapes.  Make
sure there are no entities on hidden layers.  Convert text to shapes
and keep only outlines.

Also, there may be a way in Illustrator to change splines to simething
more friendly.  That, or just brute-force redraw in Illustrator.

Worst case scenario: Ghostscript can convert the PDF to TIFF or BMP,
and you trace.

Seth Renigar wrote:
> I am doing a project now for a customer that wants his logo embossed
on the
> part.  He gave me with a .pdf file of his logo.   It is basically
very fancy
> text with lots of loopity-loops and such.  I need to get this logo
into a
> sketch so that I can extrude it.
>
> I first tried to save it as a graphics image and use WinTopo to
create the
> geometry.  This failed.  The geometry wasn't even close to being
usable.
>
> I then called the graphics designer directly.  She uses Adobe
Illustrator.
> She told me that she could export it as a .dxf or .dwg though she had
never
> done this before.
>
> The first attempt produced nothing but crosshatch when opened in
AutoCAD,
> and absolutely nothing when imported into SolidWorks.
>
> She found some export settings or something and re-exported.
>
> This time it opened perfect in AutoCAD, but only about 50% of the
entities
> (splines) would import into SW.  I got this error message:
> Entity not imported, type Spline, Handle: 8C
> Entity not imported, type Spline, Handle: 86
> Entity not imported, type Spline, Handle: 7F
> Entity not imported, type Spline, Handle: 79
> etc.
> etc.
>
> I know nothing about Adobe Illustrator.  And she knows nothing about
> exporting it to CAD.  Does anyone know of a way that I could get this
done?
> I am all out of ideas.
>
> TIA
> --
> Seth Renigar
> Emerald Tool and Mold Inc.
> (Remove "SpamFree_" from my address)

>> This time it opened perfect in AutoCAD,


Ok, from acad, save it as an R12 DXF

Now open the DXF in *Notepad*
Search down from the top of the file for the word "ENTITIES" ,
without the quotation marks.

There will be 3 lines before it:
  0
SECTION
  2

erase every line ABOVE THAT ZERO to the beginning of the file
(starting with "ENDSEC" in the line above the sero.)

Save and retry reading in with your fav cad or cam app.

What I do is,.. open the *.ai or *.pdf in Rhino3D (you can download the
free version, 25 saves) and export it as a DXF, IGES or STEP (depending
on the need).
(and, while I'm in Rhino3D I usually position/orient/scale and clean up
the sketch if need before export)

...


-- 
Posted via Mailgate.ORG Server - http://www.Mailgate.ORG

Man!!!  All these possible solutions, and I have since gotten temporarily
pulled off this project to work on a different hot, hot project.  I will
give some of these a try in the next day or two.

Thanks to everyone for your suggestions.

-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)


"rocheey" <rocheey@hotmail.com> wrote in message
news:7591268e.0410201012.2213a7f4@posting.google.com...
> >> This time it opened perfect in AutoCAD,
>
>
> Ok, from acad, save it as an R12 DXF
>
> Now open the DXF in *Notepad*
> Search down from the top of the file for the word "ENTITIES" ,
> without the quotation marks.
>
> There will be 3 lines before it:
>   0
> SECTION
>   2
>
> erase every line ABOVE THAT ZERO to the beginning of the file
> (starting with "ENDSEC" in the line above the sero.)
>
> Save and retry reading in with your fav cad or cam app.

Just to let everyone know,

Brian Mears helped me out with this problem by taking the Adobe Illustrator
(.ai) file and running it through a program called Bezarc.  It produced
perfect CAD data without a single spline in the geometry.  Instead, the
sketch consists of lines and arcs only which simplifies the data a LOT and
still looks just like the logo.

From what I have seen, I am going to purchase a seat of Bezarc.  If you also
have a need to get data from an Illustrator document, I highly recommend it
for you as well.

I would like to thank everyone again for your input and ideas.  I am sure
that several of these solutions would have worked to some degree or another.
But I doubt any of them would have produced better quality than Brian did
with the Bezarc program.

This group is great!
-- 
Seth Renigar
Emerald Tool and Mold Inc.
(Remove "SpamFree_" from my address)


"Seth Renigar" <SpamFree_srenigar@SpamFree_emeraldtoolandmold.com> wrote in
message news:T0ddd.27740$zA3.4400969@twister.southeast.rr.com...
> I am doing a project now for a customer that wants his logo embossed on
the
> part.  He gave me with a .pdf file of his logo.   It is basically very
fancy
> text with lots of loopity-loops and such.  I need to get this logo into a
> sketch so that I can extrude it.
>
> I first tried to save it as a graphics image and use WinTopo to create the
> geometry.  This failed.  The geometry wasn't even close to being usable.
>
> I then called the graphics designer directly.  She uses Adobe Illustrator.
> She told me that she could export it as a .dxf or .dwg though she had
never
> done this before.
>
> The first attempt produced nothing but crosshatch when opened in AutoCAD,
> and absolutely nothing when imported into SolidWorks.
>
> She found some export settings or something and re-exported.
>
> This time it opened perfect in AutoCAD, but only about 50% of the entities
> (splines) would import into SW.  I got this error message:
> Entity not imported, type Spline, Handle: 8C
> Entity not imported, type Spline, Handle: 86
> Entity not imported, type Spline, Handle: 7F
> Entity not imported, type Spline, Handle: 79
> etc.
> etc.
>
> I know nothing about Adobe Illustrator.  And she knows nothing about
> exporting it to CAD.  Does anyone know of a way that I could get this
done?
> I am all out of ideas.
>
> TIA
> -- 
> Seth Renigar
> Emerald Tool and Mold Inc.
> (Remove "SpamFree_" from my address)
>
>
>