I am tring to represent wire mesh in SolidWorks. If I try to do this by using a solid cut that is patterned then there will be thousands of cuts. My system won't handle that. I am a previous Pro/E user and had the same problem then. I never found a solution. Thanks in advance for any help.
Do other systems handle this cut? If so, the problem is with your system. You may need more RAM or a better system.
If other systems can't handle this cut, then you may have encountered a limitation in pattern calculations or openGL triangles. You should then report this to your SolidWorks reseller.
My computer is not the problem. It's a Dell Precision Workstation (P4-2ghz, 512mg of ram, SCSI hard Drive and nvidia graphics card). I can create complex helical sweeps, complex assemblies and anything else, except expanded metal. The number of diamond shaped cuts is approx 50,000. If anyone’s computer can do this as solid cuts successfully, then please let me know how. This is 26ga flattened expanded metal with 60%open area. It doesn't need to be true features (if that's possible). It is for a presentation of a product concept. In a 2d package like ACAD it is done with hatching, or fill patterns.
How detailed do you want this? If you just want a simple representation that consists of a thin sheet with a ton of square holes that is one thing. If you want something that looks like a woven wire mesh that is another. I looked in the model library area of the SWX website and found nothing.
To model the screen using either of these techniques the work is not difficult. However, if you are experiencing long regen times as a result of the many features then I would suggest you make a large screen as its own part and then save it as a parasolid. This will make it a very detailed, dumb, fast part that you can then pull into an assembly and cut to size. (Sort of like the real world. Cool!)
Before we come up with a solution perhaps you can fill us in as to what you require.
I just created a wire screen part that uses a design table to control the following: Wire Diameter, Pitch and Grid Length/Width (in number of pitches). I used a sweep that resembles a simple rise and fall cam with the ends and middle of the path curved with a radius that matches the pitch of the mesh. Then I used a circular pattern with 4 instances of this sweep at 90 degrees to create the first grid square. A linear pattern is then applied to this circular pattern to make the large sheet.
I also have two other parameters controlled by equations within SWX, the intrusion depth and the spacing for the linear pattern. The intrusion depth assures that the wires intrude into each other's space so that there are no disjoint bodies (set to 10% of the wire diameter). The linear pattern dimension is two times the pitch of the first grid. (This is clearer once you see the model.) I used a square mesh so there are a couple of linked values.
I am sending this file to the SWX model library. It makes a large file so I don't want to be e-mailing it, please. Due to its large size I suggest that to really use this file you open it all by itself, set the parameters you want for a given configuration, and then save that part out as a parasolid. Use that parasolid for your application and cut it down as if you were cutting a roll of screen wire. Your modeling will be much faster and you probably don't really need the screen part to be paramtric anyway, maybe just its trimming needs to be parametric.
Since you have used hatching in AutoCAD in the past, why not just use hatching to represent the wire mesh on the SW drawing and not worry about it on the solid model? SW has quite a few hatch patterns and there is probably one that would at least be good enough to get the point across.
Unless you're the guy who is designing the mesh - yours is the company who manufactures the mesh - I don't see why you need that much detail. I would suggest slappng a thin slab in there and make it transparent - so you can see thru it. Then add your specific purchase data in the $PRP@DESCRIPTION, so it'll show-up right in your BILL OF MATERIALS. Finite details are real nice to have, but in most cases, detail like this will print as a black blob anyway. I hate to say it, but at the end of the day, most of us are still making pretty pictures with important numbers on them. Gee, do I sound jaded?
You can also cheat this problem by using a decal of a wire mesh if you are doing this for a presentation and have PhotoWorks... you just won't be able to see through the decal.
Also, if you search comp.cad.solidworks newsgroup you should be able to find an example of a wire mesh (they called it a "bowl" I think) fan shroud that was discussed about 1.5 months ago. It might be of some help.
Again on Photoworks, you can get a see-though mesh if you use a mask in the decal. the mesh material that comes with solidworks makes proper looking meshed materials so it should be possible to manage by making a bitmap of your diamond cut-out.
however depending on the complexity of the rendering you need to do, the one limitation is that it will not really look that 3d up close, just like a very thin mesh of foil. tips to render it properly, turn off the "apply solidworks properties" in the photoworks setup if its on... and modify you lighting to throw shadows through transparent objects.
If your object is flat surfaced, i.e. non-cylindrical, and it's a square mesh; generate a cross hatch in the desired drawing view, and change the hatch to ANSI37 (Lead,Zinc, mg). Adjust the scale and angle to suit.
Here is an interesting technique that allows a decal to be placed on a surface in such a way that the decal can be seen through in places. I haven't had a chance to fully examine the method, but the rendering looked convincing.
You can do this with Face curves. Select a face, go to Tools/Sketch Tools/Face curves, adjust the mesh and click okay. Unfortunately you have to do this for every single face you want to be represented as "wireframe".
Now that you have converted (= copied) all faces I suggest that you put all the resulting 3D sketches in a folder (if you havn't updated to SW2003 I'm sorry, you have to leave them in the featuremanger), make another configuration where you hide the solid body so you can only see the wireframes. In your standard configuration suppress all wireframes-sketches (for obvious performance reasons).
I havn't figured out if I can upload an image or example ZIP files here, so I hope my explanation was clear enough.
I had to make a screen a while ago that had to fit on the inside of a cylindrical surface. I needed to be able to detail the part for production but I was not worried about displaying the weave of the wire. I made a square sheet metal part that was about 3/4" bigger than the hole it was up against and had a radius that fit on the inside of the cylinder. Then flattened it out and removed all but 1/4" from all edges. I added 2 more sketches to the front and side. Each contained a .025 dia. circle located with an array of additional fixed circles .075 apart that were extruded to the opposite face. A final cut removing everything outside the diameter I needed creating the finished part. This was a very fast process and does not seem to take up all that many resources. It looks right unless you are zoomed in very close to the wire. I did try creating the same part with the wire woven in place. The two sweeps didn't take all that long but when I did the first of the 2 linear patterns needed, it took over 2 hours and the memory reported by the Task Manager jumped up to over 789,000k. I didn't bother going any further with it.
Just if you are curious: I set a a page at one of my websites with a screenshot and a example file for download (SolidWorks 2003 format) with a "wireframe" model. I hope I understand it correct and this is what Chris was looking for.
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RE: How do I represent wire mesh in SolidWorks?
Do other systems handle this cut? If so, the problem is with your system. You may need more RAM or a better system.
If other systems can't handle this cut, then you may have encountered a limitation in pattern calculations or openGL triangles. You should then report this to your SolidWorks reseller.
cheers,
Joseph
RE: How do I represent wire mesh in SolidWorks?
But if your system can't handle what you described above you may not be able to handle a few helixs.
Regards,
Scott Baugh, CSWP
3DVision Technologies
credence69@REMOVEhotmail.com
http://www.3dvisiontech.com
http://www.3dmca.com
*When in doubt always check the help*
RE: How do I represent wire mesh in SolidWorks?
The number of diamond shaped cuts is approx 50,000. If anyone’s computer can do this as solid cuts successfully, then please let me know how.
This is 26ga flattened expanded metal with 60%open area.
It doesn't need to be true features (if that's possible). It is for a presentation of a product concept.
In a 2d package like ACAD it is done with hatching, or fill patterns.
Chris
RE: How do I represent wire mesh in SolidWorks?
To model the screen using either of these techniques the work is not difficult. However, if you are experiencing long regen times as a result of the many features then I would suggest you make a large screen as its own part and then save it as a parasolid. This will make it a very detailed, dumb, fast part that you can then pull into an assembly and cut to size. (Sort of like the real world. Cool!)
Before we come up with a solution perhaps you can fill us in as to what you require.
- - -DennisD
RE: How do I represent wire mesh in SolidWorks?
I also have two other parameters controlled by equations within SWX, the intrusion depth and the spacing for the linear pattern. The intrusion depth assures that the wires intrude into each other's space so that there are no disjoint bodies (set to 10% of the wire diameter). The linear pattern dimension is two times the pitch of the first grid. (This is clearer once you see the model.) I used a square mesh so there are a couple of linked values.
I am sending this file to the SWX model library. It makes a large file so I don't want to be e-mailing it, please. Due to its large size I suggest that to really use this file you open it all by itself, set the parameters you want for a given configuration, and then save that part out as a parasolid. Use that parasolid for your application and cut it down as if you were cutting a roll of screen wire. Your modeling will be much faster and you probably don't really need the screen part to be paramtric anyway, maybe just its trimming needs to be parametric.
- - -DennisD
RE: How do I represent wire mesh in SolidWorks?
RE: How do I represent wire mesh in SolidWorks?
I would suggest slappng a thin slab in there and make it transparent - so you can see thru it. Then add your specific purchase data in the $PRP@DESCRIPTION, so it'll show-up right in your BILL OF MATERIALS.
Finite details are real nice to have, but in most cases, detail like this will print as a black blob anyway. I hate to say it, but at the end of the day, most of us are still making pretty pictures with important numbers on them.
Gee, do I sound jaded?
tatej@usfilter.com
RE: How do I represent wire mesh in SolidWorks?
Also, if you search comp.cad.solidworks newsgroup you should be able to find an example of a wire mesh (they called it a "bowl" I think) fan shroud that was discussed about 1.5 months ago. It might be of some help.
"The attempt and not the deed confounds us."
RE: How do I represent wire mesh in SolidWorks?
the mesh material that comes with solidworks makes proper looking meshed materials so it should be possible to manage by making a bitmap of your diamond cut-out.
however depending on the complexity of the rendering you need to do, the one limitation is that it will not really look that 3d up close, just like a very thin mesh of foil.
tips to render it properly, turn off the "apply solidworks properties" in the photoworks setup if its on...
and modify you lighting to throw shadows through transparent objects.
RE: How do I represent wire mesh in SolidWorks?
RE: How do I represent wire mesh in SolidWorks?
http://www.mikejwilson.com/solidworks/files/x-ray_vision.zip
The server seems to be quite busy sometimes, so downloading sample parts is sometimes slow.
Jeff Mowry
DesignHaus Industrial Design
http://www.designhaus-i-d.com
RE: How do I represent wire mesh in SolidWorks?
You can do this with Face curves. Select a face, go to Tools/Sketch Tools/Face curves, adjust the mesh and click okay. Unfortunately you have to do this for every single face you want to be represented as "wireframe".
Now that you have converted (= copied) all faces I suggest that you put all the resulting 3D sketches in a folder (if you havn't updated to SW2003 I'm sorry, you have to leave them in the featuremanger), make another configuration where you hide the solid body so you can only see the wireframes. In your standard configuration suppress all wireframes-sketches (for obvious performance reasons).
I havn't figured out if I can upload an image or example ZIP files here, so I hope my explanation was clear enough.
Bye,
Stefan
--
unofficial german SolidWorks helppage
http://solidworks.cad.de
Shareware, freeware, tools and macros
http://swtools.cad.de
RE: How do I represent wire mesh in SolidWorks?
I made a square sheet metal part that was about 3/4" bigger than the hole it was up against and had a radius that fit on the inside of the cylinder. Then flattened it out and removed all but 1/4" from all edges. I added 2 more sketches to the front and side. Each contained a .025 dia. circle located with an array of additional fixed circles .075 apart that were extruded to the opposite face. A final cut removing everything outside the diameter I needed creating the finished part.
This was a very fast process and does not seem to take up all that many resources. It looks right unless you are zoomed in very close to the wire. I did try creating the same part with the wire woven in place. The two sweeps didn't take all that long but when I did the first of the 2 linear patterns needed, it took over 2 hours and the memory reported by the Task Manager jumped up to over 789,000k. I didn't bother going any further with it.
Lee
RE: How do I represent wire mesh in SolidWorks?
The link is http://swtools.cad.de/stuff.htm
Bye,
Srefan
--
unofficial german SolidWorks helppage
http://solidworks.cad.de
Shareware, freeware, tools and macros
http://swtools.cad.de