logo artwork in cad mold tooling 4

[triage]

We have a IGS cad file for a plastic cover plate component to be injection mold mfg.

We also have a jpg file for logo artwork which we would like as an expression (positive) image on the plastic component. The jpg is black and white. Where the image is black, we would like raised on the plastic cover about .020". I believe that the mold would then have to be cut down ~.020" deeper from the cover's surface where the image is black.

The mfg is making the mold tooling and has requested that the jpg be merged into the igs cad file.

Can anyone provide the steps to undertake or is there a different technique?

 

[Eltron]

There are a couple of ways to do this. You can import the jpg into a sketch (Tools/Sketch tools/sketch picture) and sketch over the logo. You can use the autotrace function (although I wouldn't recommend it). You can insert the jpg as a logo in PhotoWorks then trace over it.

It's a little more complicated that that, but I hope you get the idea.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[Theophilus]

There are also some third-party add-ons that will do the tracing work for you--but they need well-defined contrasts to work properly, and you might ultimately find yourself building a sketch over the results those add-ons provide anyway.

I've always inserted the bitmap image in a sketch, closed the sketch, started a new one, and traced over it with the SW sketch tools. Then copy the sketched logo sketch, paste it where you need it, scale/rotate it with the scale/rotate sketch tool, and extrude a cut or boss (whichever) to create the logo where you need it. Save the traced logo as its own part file so you can simply copy or modify it anytime in the future.



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[ctopher]

The process that Jeff describes has always been how I do it and the machine shop/molding departments can use it.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[triage]

Thanks very much for the production info:Eltron, Theophilus and ctopher!

I have found a software tool which will convert an image file to DXF. Would this make sense to use, then make the separate part file from this cad file.

Finally, merge the plastic component CAD and new dxf logo into a 3D CAD output file to be used for making the mold?

 

[Theophilus]

DXF output can be tricky stuff. I've found many times when this is done (by whatever means) the DXF comes in as chopped straight line segments--and I ultimately end up tracing everything manually anyway. So your mileage may vary with this application--who knows, it might work and it might actually use arcs that remain tangent to surrounding segments (although I've never seen it happen).

If it doesn't work, you may need to use the manual methods illustrated above.



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[ctopher]

The one problem I have had using logo's on parts is laser marking or etching can't be read from the part. It had to be programmed manually withing the laser controller, or export a separate drawing as DXF.

We could never get it to work from a part.
Also, you have to look at the tooling used to machine the logo, if machined. The radius of the tool may be too big.

For molding, it's usually not an issue.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[Theophilus]

For tooling, I always use an extruded cut or boss to create the literal logo features within the part file. If the logo contains fine detail, it's often added by EDM electrode to remain crisp without loss of ball-end mill radius.



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[kchan711]

This is very interesting. I have quick question to add. Why wouldn't you (Eltron or anyone else) recommend using Autotrace? With that said, is Solidworks 2009 better suited at accepting images than 2008 (or earlier) and is there a preferred image format?

Thanks,
Kyle

Kyle Chandler

http://www.chiefengineering.net

"To the Pessimist, the glass is half-empty. To the Optimist, the glass is half-full. To the Engineer, the glass is twice as large as it needs to be!"

 

[CorBlimeyLimey]

SW08 and 09 can import .ai (Ilustrator) files. That would be my preference.

Autotrace is OK if the logo or image has clear and distinct colour separations (contrasts).

 

[Eltron]

The autotrace function just doesn't seem to pan out very well, and if you have multiple colors or faded edges it doesn't really work at all. Unless you're going for a third-grade scribble interpretation of your image.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[triage]

Thanks everyone for your contribution.

The image which we intend to emboss to the cover is high contrast (sharp edge) black and white. We only want to raise the areas defined in black and are in process of making a sketch file per instructions above.

I feel that we can then set its z height, relative to the component surface to get the emboss height we desire.

I like the suggestion of making it a separate cad file which can be run on the tooling mill separately. We will also make a merged version in case.

I would call this issue resolved and once again thank you all for your invaluable contribution.
Regards,
Rj

 

[rfus]

I like using sketch blocks for this purpose. We will mold Designed in USA, Made in China, FCC, CE, Voltage/current, WEE trashcan, RoHS, Model, Make, company name, logo, etc all into the plastics. We usually go for a 30mil height that is burned into the tool via electrode. When possible, I will get the ai files, as CBL mentinoed, of certain things if they are vectors, and import them. It is important that AI files are saved without compression checked, or SW can't read them. They also shouldn't be saved in the latest format. AI10 is good. Once brought into SW, they are used to create a sketch block. Upon the sketch blocks insertion into the part, they can be easily placed and scaled, and then used for the extrusion, or cut extrusion. One final note is that they have to be vector based images in the first place to really use AI (i use CS2)

If not a vector based image, Creating a new part, inserting a sketch picture and tracing it, and then creating a block out of this sketch is another good way to go. Like the others said, images in jpeg comression is what you will often find, and these don't work well with auto trace because the edges have been reduced to array approximations of what the were originally were. Edges where black meets white, becomes gray. These are also horrible for use in decals because you can't image mask them.

I do like dxf. It has a special place in my heart, but they must be of good quality. Importing dxf into a SW drawing with convert to SW entities is the best way to go, and then copy pasting into a part, and converting to a block works well. If you have a lot of experience using dxf stuff, you know how to get the good stuff.

On a final note, once you burn something into a tool, It can be a pain to get out. Keep that in mind if you are going to use the plastics for different things or future products. Putting the model number seems like a good idea, but when you create the next spin of the product, you'll have to weld/fill/and polish the tool to update it, and then you can't make parts for the old model. Stay generic as possible.

too much time on eng-tips today. i really have a ton to do.

rfus

 

[triage]

great wisdom, thanks rfus!