Moving Sketch Entities

[arun17]

Dear friends,
(1)I am having some autocad drawings, from which I want to generate Solid works parts. I want to use the dwg files to make the sketch directly. How it can be done.
(2) Is it possible to move a sketch entity in a particular sketch to another sketch.
Thanks

"Knowledge is power"

 

[BBJT]

If you are using 2003 you can copy and paste directly form AutoCAD to SolidWorks. You can then use those sketches for your feature creations.

There is also a too called 2d to 3D that mat help you out. For info go under the help pulldown, select SolidWorks Help Topics, make sure the index tab is selected at the top, know you should see 2D to 3D conversion. It will walk you through the steps.


BBJT CSWP

 

[SBaugh]

You can copy it like BBJT suggested or you can bring your DWG in as a part in SW. File\Open\(change type to DWG)\ highlight the file and click Open

From there you get a menu. Pick Import as part, turn off the layers you don't want to show (dimensions, etc...) click next, adjust any options there and click Finish.


To make it as a solid follow BBJT's suggestion on the 2D to 3D. That's your only choice, because that's the only way to make a 3D model from imported 2D.

Regards

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

As BBJT said, import the AutoCAD dwg's directly into SW, and hen use the 2D to 3D tools. You can find these tools on the 2D to 3D toolbar.

The 2D to 3D tools will enable you to move the imported AutoCad sketch, as well as break the AutoCAD sketch views off and reorient and reposition them. If you are current with your support, perhaps you can pay a quick visit to your VAR for a demonstration.

When using this tool, I highly recommend that the AutoCAD imported sketch only be used as control line. Do not use the imported sketches directly for solid geometry sketches. Use secondary sketches and reference the control sketches with constraints and by using "Convert Entities".

Good and evil: wrap them up and disguise it as people.

 

[SBaugh]

I disagree Tick. I always use the imported sketch lines and it always works fine for me. I kind of defeats the purpose of importing them in if you don't use them. Plus you will have 3 extra sketches that your extrusion will be dependent on if you convert the sketches.

I would use the imported sketches. That's why you turn off certain layers so it's not seen when importing the DWG as a part. If you do bring in extra stuff like a dimension or anything you can delete so your left with just the sketch or sketches that you want to extrude. Also use "Contour Selection" when making the extrusions. See the help on that. It is extremly helpful when making 2D to 3D files.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

Actually, most of my models are based on using control line sketches. Making one or two control line or "skeleton" sketches makes for a more robust model which is more adaptable to unforseen change requests. This is especially important when working with industrial design or in support of off-site clients who do not always include you in the discussion before mandating a change.

Also, many times AutoCAD 2D view projections do not match each other exactly. Also, soetimes there are overlapping or broken lines, and the repair utility does not always fully complete the task. Another reason is to maintain the integrity of the original data, in case there are any questions about it at a later date. Lots of reasons! As far as a couple or two extra sketches, es macht nicht.


Tick says:
The true test of mettle for a CAD designer is not what he can make, but what he can change. A little forethought and a sound foundation make for a model that can withstand the inevitable changes of the design process. Remember, it's not about the model, it's about the design.

Good and evil: wrap them up and disguise it as people.

 

[SBaugh]

Actually, most of my models are based on using control line sketches. Making one or two control line or "skeleton" sketches makes for a more robust model which is more adaptable to unforseen change requests.

That's works great for you, I'm glad. I don't use skeleton sketches, but yet my models are robust and easy to change. You can make robust models without doing it like that. You can link values between dimensions, configurations, DT, etc...

Also, many times AutoCAD 2D view projections do not match each other exactly.

Thats why you use 2D to 3D so you can match them up correctly. If someone built it wrong in AutoCAD than thats the chance you take if you want to use an AutoCAD drawing. But if the user were to auto dimension it. Then the user could fix the deviation between the sketches. or if the user could just build it in SW and completely avoid all this hassle. It's better to just re-build it in SW IMO, instead of going through this combersome mess.

Also, sometimes there are overlapping or broken lines, and the repair utility does not always fully complete the task.

I have dealt with some very nasty files (especially 2D to 3D models). I have always used the AutoCAD sketches and I don't have a problem with them. The "Check sketch for feature" works pretty flawlessly for me, or if you re-built it you would have any these issues.

Another reason is to maintain the integrity of the original data, in case there are any questions about it at
a later date.

You should always keep the original AutoCAD file.

If you convert the sketches the converting is going to be the same as the original. Whats the purpose of having the original then? You can't control a converted edge unless you either break the references or move the parent? if that's the case keep the DWG, don't convert the sketches, and use the originals.

Lots of reasons! As far as a couple or two extra sketches, es macht nicht.

huh?

Tick says:
The true test of mettle for a CAD designer is not what he can make, but what he can change. A little forethought and a sound foundation make for a model that can withstand the inevitable changes of the design process. Remember, it's not about the model, it's about the design.

I realize that, do you not think I don't know that?

arun17,
One thing I forgot to mention after you insert the 2D geometry is to do an "Auto Dimension" this away you can control and have "Design intent" for future use.

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

to SBaugh:
I was certain that you did know that. The last bit was only a bit of street-preaching shouted out among the general SW public. Hence, the "Soapbox" emoticon.

While we tend to disagree on the finer points, believe me when I say I hold you and your opinions in high regard, even if they differ from mine. You are clearly competent and talented, and I would never dare say otherwise.

As far as my approach goes, it is borne from hard lessons learned and not forgotten.

Good and evil: wrap them up and disguise it as people.

 

[LoveAeris]

I have SW2003+SP3.1 on W2K.

Some manufactures have online CAD data and some are DXF/DWG format. You can make a solid model as follows from the format instead of Copy&Paste.

1. Open DWG from SW.
2. You get a dialog box and select "Import to part" and you can go through or hit "Finish"
3. As soon as the conversion is done, you are in Sketch Mode. Right click on a graphic area and select "Contour Select Tool"
4. Select lines or whatever you need to extrude.
5. The converted sketch is still available to make multibody. Right click on a graphic area and select "Contour Select Tool" again. (make sure the sketch is not hiddden.)

I love "Contour Select Tool" and multi-body function very much.

 

[SBaugh]

I appreciate your reply! I thought you were soapboxing me. I didn't realize you were are street preacher ;-)

I agree we do have some different opinions about this subject, but either way we get the job down and maybe arun17 can understand there is more than one way to skin a cat in SW.

I do apologize! Sometimes Tech support can get to a person...depends on the calls you get...I think you catch my drift.

Best Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[APPENG]

Good stuff guys but getting back the very first post..

You can copy stuff to new sketches using the 2d-3d toolbar yes.. but if you want to copy certain parts of sketches, you can also use the cut and paste method as well.. edit the old sketch select what you want edit/cut (or copy) and edit paste it in a new sketch..

if you have a sketch from autcad and you create a new part out of it, you want to move the sketches around as well.. hard to do by just dragging.. you wind up distorting the sketch because there are usually no dimensions or relations. so for this you can also use the TOOLS/SKETCH TOOLS/MODIFY command.. look that up in help and see if that will help you as well.

Regards,
Jon
jgbena@yahoo.com