Trim around text

[scarr]

Hi,

I have a sketch that has lots of random lines on what will be a A4 sheet, I want to place text over these lines and then trim away the ones that intersect the text, how do I do this?

Steve

[Glenn Schroeder]

Hello, and welcome to the forum. Please clarify what you mean by "random lines." If you mean model edges, then I'm not aware of any way to hide them where they interfere with the text, except by using the "convert entities" sketch function to reproduce them where you want the lines, and then hide the actual lines.

[DanPihlaja]

About the only way that I know if is to get creative with crosshatching a solid area to represent your white masking of the background of the text. Saving that as a block with the text in it and using that.

[scarr]

I have atached a screen shot that hopefully helps.

[matt]

You could explode the text into sketch elements, but that's messy. No, it's Messy.

I would avoid doing it in sketch. Use the text to make solid geometry, and then use the line sketch to break up the solid text into bodies. You can probably still get where you want to go using that method.

[Glenn Schroeder]

Will this work for you? Sketch a rectangle around the text, use the Trim tool to remove the lines inside the rectangle, then delete the rectangle.

[zxys001]

Hi,

I have a sketch that has lots of random lines on what will be a A4 sheet, I want to place text over these lines and then trim away the ones that intersect the text, how do I do this?

Steve

One way you may be able to do this is to create a Broken-Out Section (solid... but maybe you have imported lines?)?

hmm... maybe create Block (with text) to mask/obscure?

[bnemec]

What is your end goal? As matt mentioned, this might be better done working with solid body(ies) than 2D elements.

[scarr]

What is your end goal? As matt mentioned, this might be better done working with solid body(ies) than 2D elements.

Thanks everyone so far...

These are laser cut lines, I am trying to get a broken glass effect with text (not broken) in it. the resulting sketch will be saved as dxf and then into
inkscape for changes of colour so the cutter software works.

It does seen stange that solidworks dosn't treat text edges the same as other lines, I'm certainly no expert but love solidworks and find you can do most things with it.

[DanPihlaja]

Thanks everyone so far...

These are laser cut lines, I am trying to get a broken glass effect with text (not broken) in it. the resulting sketch will be saved as dxf and then into
inkscape for changes of colour so the cutter software works.

It does seen stange that solidworks dosn't treat text edges the same as other lines, I'm certainly no expert but love solidworks and find you can do most things with it.

You can dissolve the text, and then it will treat it like normal lines. But that is a one way process.

[sergio.monti]

Other solution could be to extrude the text - therefore you get a solid and the sketch text will be hidden - then edit the sketch containing the lines and use 'Convert Entities' command selecting the top surface of the text. You are then able to cut inner lines.

[SPerman]

I think Matt's suggestion of using solids is the best, if I am understanding what you are looking for. Personally, I would do this in an assembly with the background as one part and the text overlay as another. Attached is an example as a multibody part. The "broken glass" feature needs a better solution. I think your geometry would perform better than my random collection of criss-cossing lines.

[scarr]

I think Matt's suggestion of using solids is the best, if I am understanding what you are looking for. Personally, I would do this in an assembly with the background as one part and the text overlay as another. Attached is an example as a multibody part. The "broken glass" feature needs a better solution. I think your geometry would perform better than my random collection of criss-cossing lines.

I think your version of SW is newer as it fails to load in my very old version (2010) :-(

[bnemec]

Solid modeling software works best working with solids. Sketches are for the sake of making solids (at least in history based parametric modeler). Extrude the text as one body, extrude the rest of the block as another body, use the random lines as curves to split the face of the block (will not split the text body). copy the text body and use the copy as a tool to cut from the main block (gets rid of the lines where the text would be). Boolean add the original text body to the main block body. What I'm not 100% certain about is if saving the model as dxf will get those split face lines or not. I could try it, but I'm guessing your version might behave differently than what I have.

[JSculley]

Thanks everyone so far...

These are laser cut lines, I am trying to get a broken glass effect with text (not broken) in it. the resulting sketch will be saved as dxf and then into
inkscape for changes of colour so the cutter software works.

It does seen stange that solidworks dosn't treat text edges the same as other lines, I'm certainly no expert but love solidworks and find you can do most things with it.

Here's an efficient way to do this:

1. Extrude your text

2 Sketch and extrude a super-thin rectangle that runs through the text joining the letters together into a single body

3. In your lines sketch, use the 'Trim away inside' option of 'Power Trim'.

You select the single front face (thanks to the sketched rectangle extrusion) and then click and drag (top right to bottom left) a selection box around all the sketch lines at once. SW will think for a bit and then trim away all the line segments inside the face:

4. Use a Delete Body feature to eliminate the solid, show your original text sketch and you're done-ish.

I say done-ish because there will be some gaps in the lines anywhere they cross the thin rectangle that you may want to clean up but the laser will probably blend them together anyway.

[len_1962]

see pic has the instruction on it.

using solids saves alot of time, sketchs are not always the fastest way to get stuff, features baby!!

[Frederick_Law]

Do it in 3D.
Extrude different regions to different height. So you can see the edge when looking down on it.

You'll need to avoid all the ZTGs

[AlexLachance]

Thanks everyone so far...

These are laser cut lines, I am trying to get a broken glass effect with text (not broken) in it. the resulting sketch will be saved as dxf and then into
inkscape for changes of colour so the cutter software works.

It does seen stange that solidworks dosn't treat text edges the same as other lines, I'm certainly no expert but love solidworks and find you can do most things with it.

You can explode text so that it becomes lines and ellipses but then you lose the ability to modify the text.

I'd use a different layer for the broken glass effect and keep the part's outer limit with text in standard layer.

You can also do as Fred mentionned and get the desired result by extruding.

[bnemec]

...You'll need to avoid all the ZTGs

Will extruding as different bodies (uncheck the merge option) avoid the ZTGs?

[Frederick_Law]

Will extruding as different bodies (uncheck the merge option) avoid the ZTGs?

Yes, it will.

I did mine in IV, so I didn't even pay attention to ZTG

[len_1962]

Have you guys looked at my SW File?
No need to extrude different levels for the hatch pattern, just do a split face.
No need to convert text to geometry or any trimming, just extrude it tru and above the split face.
I had to make a drawing because the part file wouldn't create the DXF with the split lines but the drawing would as long as the slection was set to show all lines.
less time and frustration, I do this all the time for our Universal laser, good old model maker tips and tricks

image.png (3.85 KiB) Viewed 953 times

[len_1962]

Will extruding as different bodies (uncheck the merge option) avoid the ZTGs?

no need for seperate bodies if you extrude a solid body thru only if you cut extrude is the problem with ZTG, open my part file.

just trying to help out my fellow cheeze head

[AlexLachance]

Have you guys looked at my SW File?
No need to extrude different levels for the hatch pattern, just do a split face.
No need to convert text to geometry or any trimming, just extrude it tru and above the split face.
I had to make a drawing because the part file wouldn't create the DXF with the split lines but the drawing would as long as the slection was set to show all lines.
less time and frustration, I do this all the time for our Universal laser, good old model maker tips and tricks image.png

That is a pretty nifty way to do it also!