Hello, I am curious as to how the conversion of dwg's in solidworks over to 2d autocad works? In the past with other programs I've used it hasn't been good, and had a lot of bugs. Is it pretty smooth with this now?
can open a solidworks file.
if not that then save the SolidWorks file out as and igs file and the cadworks should be able to open that.
What I mean is, how good is the conversion process from solid work to autocad. In the past it was frought with issues, require tons of hours of drawing cleanup afterwards and many more hours if you had to make a change to the model and then redo the drawings.
It seems to work ok for me. The fonts change and they appear slightly different. I don't use AutoCAD but a co-worker does and he is able to open and measure etc all of the .DWG files I send him and doesn't complain. I take that as a good sign.
The problem is the changing fonts, and dimensions etc. My company is trying to decide wether to use solidworks. But deliverables need to be 2d autocad files, and if the conversions changes the fonts and such that won't work.
I haven't played around with it enough to see if there is a way to have a font that is supported by both and thus unchanged in translation. But they translate well in my limited experience opinion. I save the .slddrw as a .dwg using the default settings and using the proper scaling, send the .dwg, my coworker opens it and it is fully functional, and we go on with our day.
I've saved some SolidWorks drawings as AutoCAD drawings, and have found that the options selected can make a big difference. If done right they should only needed minor editing to clean up.
Cool. Are you able to, say, set parameters or "layers" within solidworks for the linework, that will then be on individual layers in autocad when you convert? for example, I have a 6" pipe in my model, when I convert my drawings from soild works to autocad, I want that 6" line to be on the layer designated for 6"lines so that it plots according to its layers plotstyle.
Jonathan Foli wrote: Cool. Are you able to, say, set parameters or "layers" within solidworks for the linework, that will then be on individual layers in autocad when you convert? for example, I have a 6" pipe in my model, when I convert my drawings from soild works to autocad, I want that 6" line to be on the layer designated for 6"lines so that it plots according to its layers plotstyle.
Jonathan Foli wrote:
I think it saves Layers, but someone else that's more familiar with AutoCAD will need to answer for sure. I know just barely enough about AutoCAD to open a drawing, print it, and close it again, and I usually can't even do that much without getting p***ed off.
WOW! I have the exact same thinking about AutoCAD. In SW's I could print drawings from it with ease. Then my co-worker would give me a DWG from AutoCAD and simply ask me to print it. I'd spend ton's of time just trying to do the simplest things ~ like print. It would make me so mad, I'd tell my co-worker the next time he'll have to buy me lunch before I go through that frustration again!
Have you tried using Draftsight? It comes with Solidworks.
In order to save and create layers, you would have to enable and utilize the custom map and create a mapping file.
2017 SOLIDWORKS Help - DXF/DWG File Mapping
I save as AutoCAD all the time.
One my customers require deliverables in AutoCad
Two the vendors who make my parts use AutoCAD
I have created a "Map File"
That when using it
it will first create in the new AutoCAD file layers that would represent All the Solidworks entities
NOTE if you look at the attached file, it is a text file, you can see that the layers I have it create all are prefixed with "SW-"
this is so I will know that any item on an AutoCAD File layer that starts with "SW-" is something that, most likely, came from Solidworks
I/It will assign a color to that/those layers
Then it will "MAP" the SW entities that I want to my layer of choice (one of the layers I/it created in the first step)
(This mapping is done when setting up the map file and can be edited later if desired)
You may have to tell SW where you put the "Map File" (ie.. Settings "File Locations")
Couple of things to set:
Enable and choose a "MAP" file
(mine is "ACADMap 04-21-16" and is attached)
Enable "Scale output 1:1"
(This is sort of important when sending say a sheet metal part as a DWG to a vendor to be made
For, in the past, I have got back a part that was 1/4 the size it should have been, I having not checked the box,
for the vendor just took the DWG file and fed it to his lazer machine)
Checking it also it makes the AutoCAD dimensions NOT be scaled Thus one can measure 1:1 in the AutoCad file
I all ways save as an AutoCAD R2000-2002 so my supplier/vendor can open it in his old version of AutoCAD
The only time I need Splines as opposed to Polylines is when I send a DWG to my EDM man to cut a gear.
(and I want a TRUE involute tooth form)
The only other draw back is the "Font File" if you open a saved DWG on the machine where you have the Solidworks you saved it from opening the DWG in AutoCAD will show you the special symbols used in Solidworks.
That is because the file it looks to is on your machine! BUT if you do not send that font file with the DWG and even if you did send it the receiver would not know what to do with it, the symbols will not show or if they do will not show the right way.
To get around the font problem --- I have modified the "calloutformat.txt" file to NOT use symbols and use text like "C'BORE" etc...
All in All I get VERY good results, Even the Tile Block comes thru in AutoCAD all anointed.
A screen Shot:
Another important point about SCALE:
set your SW drawings sheet properties here:
And always for the main view in your drawing set it to: "USE SHEET SCALE"
Doing this ensures that the AutoCAD export at 1:1 will be what you want and
will be consistent across all your AutoCAD DWG files.
Thanks Robert Conklin. That was the exactly the information I was looking for. Thanks a lot for your insight on this. There's still one more glitch which remained unresolved. After this export all the dimension are driven into numbers of dimstyles. Any minor change I try to do in these dimensions will turn them as below. Any suggestions??
This is all I know. (Well part of what I know)
The "Extend beyond dim lines:" is "Zero" even tho it shows dim lines extended. Editing this value (Here In AutoCad) for "SLDDIMSTYLE2" should change how the Dim appears in AutoCad.
I do not know why it shows extended when the value of "Extend beyond dim lines:" is "Zero"
A translator glitch. Is my guess.
Thanks Robert, but that means you have to edit all these "SLDDIMSTYLE"s in autocad??! That's a huge task!!!
A couple of things I would add to Robert Conklin 's excellent reply
If you have different scales on sheet Solidworks will pick the first (I think) created view as the 1:1 scale and any other views of different scale will be scaled up or down from that.
You will get a couple of warnings
If you have 3 views at 1:10 and one of these was created first & 1 other at 1:2,
the 3 at 1:10 will come in at 1:1 and other at will get scaled up or down depending on view scale (in this case 5x that dimensionally)
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