complex undimensioned sections - eg logo

[sdesaulles]

OK, really annoyingly I asked this before on the forum, but as there is no
method I can see to find my old posts, I can't retrieve the answer that
someone kindly gave.

So, here we go again. If I have a complex logo, or a complex pattern of
holes, how can I get a section that I can 'trace'. I know I can import a
section using 'data from file' and pull in the adobe or dxff etc file, but
then ProE, bless it, insists on trying to dimension and constrain every tiny
bit of it, eventually it all gets too much for it and it gives up.

There is a way however of getting an undimensioned 'reference' profile,
where you can then just select the bits you want to trace within sketcher -
can anyone please remind me how to do it?

Many Thanks in advance.

Stephen

 

[sohail abbas]

when you are in sketching mode delete all the rectangular referece and take theco-ordinate system as a reference, now sketch> data form file, and insert the sketch,


NOTE: create the co-ordinate system where you want to place your sketch.

 

[sdesaulles]

Hi Sohail,

I think this might work, but someone emailed me the original solution in the
meantime - take it in as and IGES file, that way ProE doesn't try to dimension
the whole thing - sometimes it just tries to be too clever for its own good -
bring back CDRS!

Thanks for the tip anyhow, I will try and see if works that way too.

Stephen.

 

[jbuckl]

I did a logo 'UDF' by importing the iges of a logo into a sketch (ie notin a part) the sketch included a vertical and horizontal centreline at the origin.


I added two dimensions to the centrelines from the desired origin edgesto the centrelines, then zoomed right in then hit 'autodim' when your zoomed in close theregeneration does not change the design. The two dimensions can be regenerated to zero and deleted after alignments have been added.(intent manger was switched off!)

 

[dibz]

HI
the best way for u is not iges. open the dwg file directly in proe as a .prt file. then very easily u can work on it without any dimension or constraints. it is very simple

 

[sdesaulles]

Hi,

Thanks for that. But how? Saving from Adobe Illustrator as a DWG, I can
then open as a drawing in ProE, but not as a part, cchanging the .dwg
to .prt certainly doesn't help me either.

Sounds like is should be easier - but can't get it to work ass described
currently.

What am I doing wrong?

Thanks

Stephen

 

[michaelpaul]

This drives me nuts as well. I wish that Pro/E would allow the ability to utilize free floating (not fully defined) sketches for instances like this. It's really a pain to have to bring in sketches from file, create a coordinate system, etc)

I usually just bring in the logo as an IGES which means I have to scale it external to my part. I create a coordinate system somewhere in the IGES and then create a CSYS in my part to orient it. Of course, it' ssometimes an iterative process to get the scale correct which is quite annoying.............

Michael

 

[dibz]

HI
when u open dwg file proe will ask u ,whether u want to open it as drawing, part, assembly file etc.
select part option.

 

[sdesaulles]

Hmm, when I do that it imports all the letters of the logo one over the top of
another - so I end up with about 12 stacked letters - which incidentally is
exactly what happend when I tried to import the DWG into the sketch as a
'data from file' to begin with. The DWG does open in other packages (eg
ashlar vellum) just fine, so it is just ProE that screws it up.

Cheers

Stephen

 

[michaelpaul]

Hmm, when I do that it imports all the letters of the logo one over the top of

another - so I end up with about 12 stacked letters - which incidentally is

exactly what happend when I tried to import the DWG into the sketch as a

'data from file' to begin with. The DWG does open in other packages (eg

ashlar vellum) just fine, so it is just ProE that screws it up.



Cheers



Stephen

I've had problems doing the same thing as well. Not necessarily for logos, but I like to bring in the silkscreen layer of a PCB to lay onto my 3d board so I know where all of my components go. That way, I can place the critical components within the silkscreened area and I know that they are exactly where they are supposed to be.

The problems I've had are when Pro opens the fild into a sketch it often times treats circles as splines and each line of a letter becomes a seperate entity. I end up with WAY too many entities for pro to have on one sketch so I spend a ton of time cleaning up the sketch to make it work. the IGES approach seems to work best but even then it's not failsafe.

Michael

 

[james.lynch]

if importing a dxf ensure that it is fully exploded (using autocad or something) -this should fix your letters overlappingproblem etc..


also... if you have advanced assembley.. create a part, import DXF or iges create your 3d part. make a solid surf copy. publish thisquilt and an appropriate coordinate sys..


now in your main part..


creat one coordinate sys for transformations (no rotations!) then create a second coordinate sys (referencing the one just created) - this second one is for rotation.


now bring in your logo using copy geom - very easy to move usig the 2 coordinate sys and to scale, simply scale your logo.prt and regen!


hopethis helps!


James

 

[Huug]

As mentioned before, logo's are ALWAYS a pain in the ass in Pro/E.

The problem with DWG/DXF is that it is usually devided in too much entities, so you won't be able to use it as a sketch.

The method I use is the illustrator/Rhino route. I ask the graphics department to outline the logo and scale it to the correct size as I want it. Than they export this Illustrator file to a legacy format, and import that in Rhino. In Rhino it can be oriented and positioned coorectly to the origin, and than export it as an IGES file.

The than easily imported IGES file (curve) in your part is of the correct size and with the correct number of entities, so it can be used for sketches and protusions.

This is the only route that I know of that copies the exact lines and
splines as in the Illustrator file, so it is not devided. The
Illustrator file should be correct also, with closed curves and no
double entities.

Futhermore: ask yourself WHY you want to import a logo.

As it should be embossed in a plastic housing part for example, you would think it should be in the 3D file. But any mouldmaker wouldn't be happy with it. They have to take extra effort to remove the logo from your file, smoothen the surface beneath it and create the cavity on the first hand with no logo. That logo is added later in the process by etching or engraving, where they normaly make use of the original *Illustrator* file! So you as a CAD designer and the mould maker are spending to much time for adding and than removing something that is of no use.

Huug


Edited by: Huug

 

[[-Skint-]]

I agree with Huug, however :


There are other reason`s other than manufacturing, people want logo`s on the models for reference, design, images, renderings etc etc so they are still very much required.


What annoy`s me sometimes, is that some people assume that everybody who has pro-e automatically has acces to Illustrator / Photoshop / Rhino bla bla bla, when realistically people do not. Shouldn`t we all be trying to improve pro-e to be able to do this all within its own software

 

[sdesaulles]

Hi, thanks for that. Interesting point re the toolmaker removing the logo
in any case. We are using ProE more as a design than specification tool in
this instance - so need to take surfaces through to Alias / 3DS for
rendering - so Logo does need to be in the part - or you end up messing
about in Photoshop.

The way I use it to create a quilt part - which is then scalable within ProE
- and can be used as a cutter within assembly.

I use illustrator and then Graphite / Vellum to do the same thing you use
Rhino for - just laundering the format.

Cheers

SStephen.

 

[michaelpaul]

]

What annoy`s me sometimes, is that some people assume that everybody who has pro-e automatically has acces to Illustrator / Photoshop / Rhino bla bla bla, when realistically people do not. Shouldn`t we all be trying to improve pro-e to be able to do this all within its own software

Yep, I only have Pro on my desktop so it's a royal PITA to have a sketch converted into something else so I can open it.

This is one of the big things that drives me insane about Pro. As some know from my previous posts, I've come back to pro from SolidWorks and in SW this operation was super EASY. all you did was open the DXF, select all of the entites, do a copy to copy them to the clipboard. then, in your new part, you create a sketch, past the entites onto the sketch, scale or reposition as necessary and you're done! Since SW doesn't require a fully dimensioned sketch, it can be placed anywhere on the sketch without a problem. it was such a simple operation and now it's just a pain.

I spent a day trying to cnovert a PCB silkscreen layer from a format the EEs used into something that I could open in Pro. it would take me 5 minutes before. Just one of the things that Pro doesn't seem to handle well.

But, I make due now and figure out a way to make it work.

Michael

 

[Huug]

] What annoy`s me sometimes, is that some people assume that everybody who has pro-e automatically has acces to Illustrator / Photoshop / Rhino, when realistically people do not.

Absolutely true. So that is why if someone (a boss, a customer) wants you to put a logo onto any Pro/E part, he should supply you with a correct IGES File, contaning only closed curves and splines, at the correct size and positioned to a coordinate system that matters. I usually pick up the phone and let someone else at a graphics department do the job.

Huug

 

[sdesaulles]

errm, right, only I am the graphics department, and the design
department, and the specification department, and IT, project management,
client liaison............

 

[Huug]

I spent a day trying to convert a PCB silkscreen layer from a format the EEs used into something that I could open in Pro.

My electronic friends supply me with DXF files from their system.
Pretty easy and allows quick checking.
Although I do put them in a separate part that I can suppress.
And sometimes they come in micrometers, so I have to scale them a factor 1000.

View attachment 2398

Huug

 

[zeta]

Me too, our PCB layout dept. provides me a DXF and let me import to into ProE for checking.

I open DXF as a ProE prt then assemble to simple protruded plate.

Open as a ProE part rather then import sketch can avoid too many unconstrained dimensions.

But when layout update, I have to update component manually. Do you have ideas? Can IDF works?