I would like to change an extruded model to a 3D line model.
Can someone tell me the process ?
Thank you,
Frank
I would like to change an extruded model to a 3D line model.
Can someone tell me the process ?
Thank you,
Frank
Let me rephrase that question:
I would like to change a 2D extruded solid model into a 3D line model.
Can anyone tell me how to do this ?
ok,.. I will stay with my same response above.
Your answer makes no sense to me. I can't understand it.
Regardless, I want to change a 2D SOLID model to a 3D LINE model.
Thank you
F. Leatin wrote:
Your answer makes no sense to me. I can't understand it.
Regardless, I want to change a 2D SOLID model to a 3D LINE model.
Thank you
I think we have a language issue. There is no such thing as a 2D solid model.
Please post some pictures, a before-and-after, etc. Perhaps those will be worth a thousand words.
..I thought I saw him in 3D,..(a fun import!)..
F. Leatin wrote:
Let me rephrase that question:
I would like to change a 2D extruded solid model into a 3D line model.
Can anyone tell me how to do this ?
I don't really understand the question.
Aren't all extruded solid models 3D models?
And what is a 3D line model. Do you mean a 3D sketch?
I'm not being sarcastic here, I truly don't understand.
Your right, all model are 3D. My mistake. But it is possible to convert a Solid model to a "LINE ONLY" model. This is what I need to know how to do.
Thank you for your response.
F. Leatin wrote:
Your right, all model are 3D. My mistake. But it is possible to convert a Solid model to a "LINE ONLY" model. This is what I need to know how to do.
Thank you for your response.
So are you trying to convert this:
To This?
Exactly correct Tony.
I'm told to draw the solid model, then select a line entity. Then "Control A", Then "Convert Entities". Then Hide the sketch and I should be left with a "Line only" solid model as your reply is showing.
But this in not working for me. I'm either missing something or ?
Solidworks Weldments tutorial steel structure - YouTube
This video gives a demo but when I follow it, it does not work for me ? Not sure why ?
Are you using selection filter edges?
Are you in 3d Sketch?
![2018-10-24 14_17_11-SOLIDWORKS 2015 x64 Edition - [Part1 _].png](https://forum.solidworks.com/servlet/JiveServlet/showImage/2-903647-443963/2018-10-24+14_17_11-SOLIDWORKS+2015+x64+Edition+-+%5BPart1+_%5D.png)
F. Leatin wrote:
Solidworks Weldments tutorial steel structure - YouTube
This video gives a demo but when I follow it, it does not work for me ? Not sure why ?
I didn't go thru the whole thing but the selection trick he showed, selecting one line then holding control and selecting the body and that supposedly selects all the lines that make up the body, didn't work for me. Maybe he left a step out.
What you can do is start a 3D sketch, hold down control and select all of the edges then click on the convert entities icon 
Close the sketch and you'll have a 3D sketch of your model. I'm not sure what you'll do with it.
Can I ask why you need this? Is it just for display? If so you can use the display mode I showed above which is exactly what Glenn Schroeder showed.
In your heads up display click the down arrow on your display style icon and select the wireframe style.
That just shows all edge of your model.
Tony Tieuli wrote:
... the selection trick he showed, selecting one line then holding control and selecting the body and that supposedly selects all the lines that make up the body, didn't work for me. Maybe he left a step out.
No steps omitted - the video instructed to Ctrl A to select the remaining edges. Worked for me.
Looks like a clever way to get a skeleton wireframe for a Weldment Frame without having to tediously sketch a 3D sketch. I like it.
J. Mather wrote:
Tony Tieuli wrote:
... the selection trick he showed, selecting one line then holding control and selecting the body and that supposedly selects all the lines that make up the body, didn't work for me. Maybe he left a step out.
No steps omitted - the video instructed to Ctrl A to select the remaining edges. Worked for me.
Looks like a clever way to get a skeleton wireframe for a Weldment Frame without having to tediously sketch a 3D sketch. I like it.
I went back and looked again and you're absolutely right. His accent got me. I had to listen to it 3 or 4 times before I got "Hold control key and press A"
Thanks for pointing that out, it'll make life easier!
The "Ctrl-a" is very clever, I did not know about it until now. Select an edge and then Ctrl-a...all edges are selected. Select a Vertex and then Ctrl-a...all vertices are selected. Select a face and then Ctrl-a...all faces are selected. Select an edge & a vertex and then Ctrl-a...all edges & vertices are selected. Good to know!
J. Mather wrote:
Tony Tieuli wrote:
... the selection trick he showed, selecting one line then holding control and selecting the body and that supposedly selects all the lines that make up the body, didn't work for me. Maybe he left a step out.
No steps omitted - the video instructed to Ctrl A to select the remaining edges. Worked for me.
Looks like a clever way to get a skeleton wireframe for a Weldment Frame without having to tediously sketch a 3D sketch. I like it.
It is. I learned about it in a class at SW World a few years ago. See my reply (with model) on page 61 of What are your most impressive tricks of solidworks, Please spread.
F. Leatin wrote:
Then Hide the sketch...
???
Looks like Paul correctly stated solution (twice).
Why, oh why, did you not reference the YouTube video in your original problem statement?
2:13 Start 3D Sketch
2:39 Select one Edge
2:42 Ctrl A to select All edges
2:57 Convert Entities
3:07 Hide Body (not hide sketch)
If you intent is not to display as Wireframe as shown by Glenn Schroeder, then please attach your *.sldprt file here.
Is your intent to create a 2D drawing *.slddrw of your 3D model?
F. Leatin wrote:
Your right, all model are 3D. My mistake. But it is possible to convert a Solid model to a "LINE ONLY" model. This is what I need to know how to do.
Thank you for your response.
The screenshot I posted above shows how to display a solid model as lines only instead of a solid. If that's not what you want then I don't know how to help without more information.
File
Save As
Save as type: Iges
Before clicking the Save button, click on the Options button
Make sure that the "IGES solid/surface entities" is un-checked
Make sure that the "IGES wireframe (3D curves)" is checked
Click on OK
(At this point, I recommend adding the word "Wireframe" to the end of the filename you are about to create.)
Click on Save
The iges file you just saved is a 3D wireframe.
I suggest taking a training class in SW.
..start a 3DSketch,.. set your selection filter to Edges,.. windows select the whole model,.. and Convert entities..
..and... Body delete the imported model...or, if you want, remove the body completely.. remove all the edge relations and then delete the imported model.