creating model from DWG

[BRENTMARINE]

Is is possible to create a 3D model from a 2D DWG by simply bringing it in as a sketch and adding depth to it? I am using Wildfire 3. I'm sure I am trying to over simplify the process but I want to avoid redrawing many parts I have previously drawn in AutoCad.

 

[ehorton]

There is a module called Autobuildz that allows you to do this. I've only seen it used so I'm not exactly sure how to get to it, but it does work.

 

[phucxoxo]

hi BRENTMARINE !


you can useDWG file as a section of 3D part. I know 2 ways to do this. in these 2 ways, in Autocad first you should copy only the section that you want to add depth to a new file. you move the sketch to the orgin X(0) Y(0). then save this file.


- The first way: in proe, you just open this DWG file as a part and star making your part.


- The second way: in autocad you export your DWG file as a IGES file. In proE, make new part, you insert a curve--> from file , andopen your IGES file as a curve, so you can do your job from these curve.

 

[arroyopr]

I had use Autobuildz and it works and is very acurate, but a little slow if you aren't familiar with it. With that said, there's other ways to do this, like is been suggested already or save the dwg as dxf import that sucker it pro-e and start sketching it, the catch is you use the use edge tool every thing will be attach to the imported copy geomerty. So pick witch is your best bet.

 

[SRINIVASANIYER1]

Autobildz yes... as far as PTC is concerned....


For me...


Start a new part... while in sketch mode...import sketch from file...open the dwg file....window select the dwg data position it.... and go on to give a depth.

 

[[-Skint-]]

I find its just as quick and easy to start the model from scratch rather than bugger about with importing detailed cad files etc... Having said that, I have imported Loads of cad files and created the parts. Make sure you dont import too much detail in one drawing though, as the Pro-e sketcher will reply with " Computer says NO ".

 

[michael3130]

I agree with skint.


One of my clients provides all their work to me in AutoCAD format which I then turn into 3D. I always redraw it. Importing it and extruding or revolving or whatever is fine until the time comes and they make a change and you have to alter it, then you're pretty well screwed unless you start over again. If I redraw the sketch I know I have total control over any changes. Yes, it takes extra time at the start but in the long run it's worth it.


Michael

 

[bwensink]

Hi All,


I have also problems with dwg/dxf's. We get company logo's in dxf/dwg. But these logo'g are build with 1000 little lines. I have no experience with Autobuildz. Can that software replace all those lines with 1? Or will those lines disapear when i use a iges file from the Autocad file?


Thanx

 

[SRINIVASANIYER1]

We get company logo's in dxf/dwg. But these logo'g are build with 1000 little lines. I have no experience with Autobuildz. Can that software replace all those lines with 1? Or will those lines disapear when i use a iges file from the Autocad file?

I am unable to understand as to why you need to import company logos for Part creation. If you mean in the drawing template...! then the answer is yes.


In case you are using the company logo for part creation, Clean up the DWG file to remove all the hatch patterns and fills and take only the boundary to extrude.

 

[jeff4136]

BRENTMARINE,


That's a wide open question. Plates, sheet metal, struct shapes, machinings, weldments, ortho prismatics only or compound angles and contours, ...? Is the user name meant to imply marine application?


I'm another 'do it from scratch' native geometry advocate.
FWIW, of course, my thoughts ...

Unless the parts are relatively simple I doubt there's much to successfully automate, but that's a moot point because the drawings are probably not an adequate, and quite probably are an inaccurate, description of the physical object and unsuitable for defining a surface brep model without varying degrees of interpretation and modification. Some drafting software geometry representations can also be unsuitable for brep model definition; i.e. a plate edge contour described by dozens of polyline segments or, even, spline curves described by a dozen or so fit points if you want to be particular.


You need the practice / experience. Even if the parts are prismatic, e.g. don't require 'advanced' modeling functions or techniques, 'capturing intent' and building robust, easily modified, reusable parametric part models (one of the paybacks on the investment in brep modeling) is a technical art form, if you will. Knowledge of the software's abilities and limitations, descriptive and problem solving skills and thought processes not cultivated by nonassociative 2D drafting design methodologies will have to be acquired and developed.


I think the pay-me-now-pay-me-later factor is significant to the decision and time spent developing 'ease of transition' tool skills is poorly invested when weighed against time spent developing geometry description / creation skills (unless you're just doing H/V rectangles and circles you'll be a while getting to the point where you can make Sketcher sing; which it can), developing sound modeling practices and gaining experience with the more standard, universally applicable, tools and methods for importing and utilizing nonnative geometry.

 

[phucxoxo]

Hi


I have the same problem likebwensink. this mean when the DWG file contain the text, when import this DWG file to ProE, the text will disapear, anybody could show me why ?! THANKS.

 

[SRINIVASANIYER1]

if you want a complete translation of DWG objects into Proe then ,,,, Import it in the DRAWING mode. If I am correct, you also have a Font Substitution option Autocad ~ proe fonts.

 

[phucxoxo]

Hi Srini !


You are right, when i import DWG in Drawing mode, allthe textare shown, buti needopen DWG in a Part mode, because i want to use it as a curve to make a new part,could you shown me another ways, THANKS VERY MUCH !!

 

[SRINIVASANIYER1]

As I said in page 1, I prefer to clean up the drawing in AutoCAD using Tools --> qselect.... To create a part using AutoCAD entities.. enter the sketch mode in Proe and then import the sketch (Proe offers window selection for complicated sketches).

 

[bwensink]

Hi SRINIVASANIYER1



I need to import the logo to put them on plastic parts. They have to be in the part to get them in the mould.





Bram

 

[SRINIVASANIYER1]

Can you post a picture of the logo? If secrecy does not permit it, make something that looks closest for the purpose of this discussion.


Generally companies, use filled logos. In such cases it is better to erase the filling (or hatch pattern), convert them into a pline. This will ensure continuity.


A picture could help.

 

[bwensink]

I can't directly put a picture here on the forum. But when you put Silentgliss logo on Google. These logo's we get in Dwg or Dxf. The text has no hatching. But Each letter is made of hundred little lines.





Bram

 

[SRINIVASANIYER1]

hmm.... Saw the logo. I would do it this way.


Start a New layer in AutoCAD. Trace out a polyline for the logo. Delete all entities lying on other layers. Save as a new file name.


Now import this file into proe.


If time permits I shall post a sample.

 

[SRINIVASANIYER1]

Ah yes... for lines.... protrusion..solid ..thin section.... especially for the wiskers and legs of the cat.

 

[bwensink]

If I had a AutoCAD station here on work I would do the smae thing. But I only have Pro/E WF2.


Any good ideas how to aproach this problem in Pro?