How do I edit "dumb" solids from ACAD

[tools4u]

I am trying to create a good case for going over to SW from ACAD (straight ACAD 2004)to work with solids. I don't see much discussion on using or editing solids created by ACAD. I am a nubie SW user when it comes to this. We have 100's of ACAD solids which I wish to convert. I have constructed a basic sheetmetal rectangle with random holes in ACAD as a test piece. I opened it in a SW (2004) then ran "featureworks" and got a great looking part. Lost in the books someplace must be ways to do these things....maybe? Just using this flat panel as an example: (1) the complete part comes in as "1 sketch" with all holes and openings extruded. (2) all the holes are fixed. (3) How do I move the part or establish the upper right "apparent intersection" of the radiused corner as the origin. (4) I don't seem able to dimension the holes on the part so I can edit their location.

Tell me.....am I mentally approaching this wrong or do I need to change my way of doing this. I feel we need to go with SW but I need to prove it. I definately don't want to start by recreating all the ACAD solids in SW.

Thanks for any help in advance
G

 

[MadMango]

You cannot do as you want with imported 2d files converted to 3d solid models. Many find it is more useful to rebuild the models in SW, though this will take longer than just importing and converting them.

Maybe there is some setting missing in Feature Works... there are others here that us it (I don't) that might be able to help you figure out it's settings and limitations.

Ray Reynolds
"Computers in the future may weigh no more than 1.5 tons."
Popular Mechanics, forecasting the relentless march of science, 1949
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[DanielGraham]

If it is coming is as one sketch then you have to edit that sketch to modify your geometry. "Fix" is a relation in SW to keep model geometry in place without the use of dimensions. You will want to delete the fixed relations and then you will be able to re orient the geometry and drive the geometry with dimensions.

Please let me know if you need more info.

Daniel

 

[davidinindy]

I'm interested in how to improve files coming from other systems also. Featureworks works to an extent.

 

[DSRT]

One way to edit Autocad created solids in Solidworks, is to use the Surface toolbar.

 

[PDMAdmin]

tools4u,

What you are observing is basically normal behavior for FeatureWorks, although I don't usually see parts coming in as one big sketch. To get around that problem, you can use "interactive" mode and map the features one at a time. As for the holes being fixed, I believe that stems from the FW option that fixes sketches. (Even if they are fixed, you can delete that relation and then dimension them.) Regardless, FW will not insert dimensions for you where none existed in the first place.

The more complicated your parts are, the less effective FW tends to be, unless you are only mapping part of the geometry. For the complicated parts, I often find that it's a more efficient use of my time to recreate the part in SolidWorks. I know that's not what you want to hear, but switching CAD packages will always cause you a little pain, no matter what you do. Your SolidWorks VAR may be willing to help you out; try asking them if you can work something out.

 

[SBaugh]

If you have one big sketch in a part, then you should be using 2D to 3D. There you can take your sketches and turn them into features.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[tools4u]

Thanks
well, this simple plate solid came in ok thru feature works..but..yes, it was showing as 1 complete sketch. I am able to pick and "un-fix" each hole individually so I can make it dim driven. Now...is there a way to do this to all entities in mass by mass selection ?? bounding box ?? multiple picks ??

Thanks again in advance

 

[SBaugh]

I don't quite follow your statement above, but from what I gathre you need to, edit the sketch and remove any relationships to the sketch. Then add dimensions as needed.

You can window select the sketch and remove all relationships. You must maintain one to the Orgin. You can use AutoDimension to dimension the sketch. Then extrude it.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[MadMango]

Using Convert Entities, you can just select a segment of a sketch you need to select, then RMB and select Chain (or whatever option it's called).

I've had to help someone that designs in AutoCAD (still) and then brings stuff into SW. I usualy import his sketch and then start a new sketch, selecting the outer most profile of the part, Convert Entities, then extrude that into a solid. Then I convert certain feature sketches (one at a time I'm affraid) until I get a group of closed sketches that I want to make into a new feature, then cut-extrude them. I repaeat the process untill I have converted all of his sketches into appropriate features.

After all is said and done, I then delete the orignal sketch and have to go back in and fix all my missing colinear & coincident mates. It's a pain, but at the end of the day I have a fully associative part. Normally I would just grab the 2d drawing and rebuild in SW, but for these particular parts, the sketches are too big and have too many features to do that (weld fixture table plat, about 250 indexing holes for other parts, 96"x48").

Ray Reynolds
"Computers in the future may weigh no more than 1.5 tons."
Popular Mechanics, forecasting the relentless march of science, 1949
Have you read faq731-376 to make the best use of Eng-Tips Forums?