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Logo in metal

G

geertdaenen

New member
Hi everybody,


I'm having a question about the cut function in the sheetmetal mode of ProE WF2:


we want to cut out the company-logo in to a metal plate and we want to do this in the future as easy as possible.
I've tried to do this with the "data from file" function in the sketcher. But when Iput the dwg-file of the logo into the sketcher, a lot of dimensions and constrains will appear (see picture below).


Is it possible to put this logo in an easy way into the sketcher, without having a lot of dimensions and constrains? (Only one dimension to scale the logo)


In other topics I wasreading something about iges-files, but I can't open an iges-file in the sketcher.


It's possible to open the dwg-file in the part and using the offset-function of the sketcher to make a potrusion, but this is not the way to cut out our logo I think.


With kind regards


View attachment 3597


View attachment 3598
 
geertdaenen,

Once you have made the sketch you can save it while in sketch mode. After that you can call up that sketch and scale it. You will still have the dimensions you originally made the sketch with plus the options to scale or rotate when you place the sketch the next time.

cheers,

M
 
The problem is: this logo is made by 2 different sketches (with the offset function). So it is not possible to save the sketch without all these dims and constrains.


Isn't it possible to import some kind of "block" as you can do in AutoCAD?
 
geertdaenen,

It is possible to import data such as a DXF that could be made using your original features in a block form. I am not sure about scaling in that event. I would still say that saving the sketches used to create the features would work, even if it is more than one. I have something that included 7 unique sketches and I import each to make seperate features. You can keep the dimensions as is in the sketch. The tool to use a sketch from a file has a control box that allows scaling and rotation. However, your references can sometimes cause a problem.

In your case you would import two sketches. Give it a try, I doubt there is an exact duplicate of the autocad method.

cheers,

M
 
magneplanar said:
geertdaenen,

However, your references can sometimes cause a problem.
Click to expand...


Gents,


If you want to go this route (and I would) then the best thing you can do to avoid the above is when you save (File>- Save a Copy) of the sketch, save it with all the references deleted. Therefore, when you insert the sketch (Sketch>- Data from File) into a new sketch it will ref to the sketched refs in the new sketch.


When you are inserting the new sketch make sure that the scale has stayed at 1.000000


Kev


EDIT


One other thing, make sure all dims are strong in the original sketch before you save it
Edited by: prohammy
 
Ooooops,


Then maybe that scale thing should change a bit
smiley9.gif



Kev
 
If you slots are all the same width, use a thin cut and just sketch one side of the cut which will reduce the total number of entities in sketcher to 28 which will make it much easier to regenerate

An alternative to saving it as a sketched section is to save it as a UDF



DB
 
hello geertdaenen





why don't you use form to do these kind of work. just make a die of your company's logo and use it where ever required.
 
geertdaenen,

make a form as a solid part with the logo you want. then you can use it wherever. when you use the form choose the appropriate surfaces to use so it cuts out instead of pressing the shape into the metal.

sanjeevkar can correct that detail

cheers,

M
 
but I don't know the Form-feature. Or is this not a feature?
Can you describe me how I can punch out a form? And which feature I have to use?
 
geertdaenen,

the "form" is a sheetmetal function. you create the sheetmetal part you want and then make another solid model part with the details of the form shape. You then align the form with the sheetmetal part using the die/punch options for form and the sheetmetal part will take on the shape of the form.
View attachment 3935
example later...

cheers,

M
 
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