I have to use diamond plate for a number of my jobs and I found that when I modeled up a sheet of it that it caused my system to drag...so I modeled up a very small portion of a sheet and had the rest of my sheet be a plain flat solid. I did the same thing with expanded metal guarding which is a similar type of mesh.
The way I made it was to create the 'pattern' or the mesh I needed, then I transform copy on the 'pattern' to create the the larger repeating pattern of the mesh/plate at the largest possible purchase size. I then removed parameters so that I had a dummy sheet of the mesh and at a smaller file size.
Finally I added 2 trims that I could 'move' to create the desired size of the final sheet used either on the walking surface of my tool, or on the guarding around the tool.
There may be other ways to accomplish this but I wasn't able to get a replicating pattern that you need and didn't want to waste a day trying to figure it out.
Probably the easiest way is to sketch the hex pattern for a small local area of one corner. Then use pattern face. But make your solid oversize and trim back the edges later if you need to have partial holes that are trimmed away.
No matter what you do this kind of detail will make your files quite large and heavy. Blowing away the parameters may help after a fashion supposing you're willing to pay that price.
I would keep one as the master copy with all parameter intact, then choosing one of the numerous possible ways, create a copy and then remove the paramters from that, at least then you will always have a master copy that you can use as a seed to create sheets/meshes of various sizes.
Best regards
Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)
Very close indeed to my own thoughts on the matter. I use a the technique of linking the body, suppressing the original, and breaking the link to achieve that effect.
Looking at the attached (honeycomb_mesh.prt) there is a parametric pattern file as I described. I have reduced the number of instances in the grid because it reduces the file size dramatically. Running part clean-up after I did this also made a big difference. I only really altered the file because it came out at 38Mb and that became too large to post here. However the pattern itself is about as parametric as one might every care to make such a thing so as in example it may be useful in itself. I'm using measurements to keep the pitch of the pattern in sync with the sketch. Altering the size of the circle in the sketch and the offset reference curve control the size and pitch of the honeycomb.
The file honeycomb_grille.prt was created using the linked body method that I mentioned above. It better than halves the original file size and because the donor file is suppressed the system can ignore it until and unless changes are required.
Making the donor file honeycomb_mesh useful again really only involves increasing the number of repetitions in the pattern and reinstating the last extrusion. Be patient it may take some processing. By all means change something and then unsuppress honeycomb_mesh in the assembly honeycomb_grille, so that you can edit the parameters of the link and by selecting the component solid to re-associate see the result in all its glory.
![[thumbsup2]](/data/assets/smilies/thumbsup2.gif "[thumbsup2] [thumbsup2]")
