How do I create a honeycomb pattern and make it staggered and stacked in layers?
Please provide some more detail of what you want to do.
Is this what you are after doing?
I have attached a part file (created in 2014) showing you how to do it.
Thank you for the reply and I am actually looking to create something that looks like the following attached image.
Hi Mike, I would like to create a honeycomb pattern that looks like the image I attached and if you look at it you can see that the top layer is one way and then there is a layer below that which is staggered and then another layer below that which is also staggered and would probably be in the same direction as the top layer so every other layer would be staggered. I would need to be able to input the number of rows, columns, wall thickness, cell size, height per layer and number of layers when all said and done and possibly in some type of script or automation program.
What would be your maximum number of
Mike - that would depend on the overall size that I need to have end design at. For instance I might need to create a circular design with this pattern and have it be a 3" x 1" but I would have the cell size be 22mm in size.
Are you looking for a part as an example or do you want to be walked through how you would do it? How proficient with Solidworks are you?
I would like to be walked through on how do to this and I am just beginning with SolidWorks 2015 edition. I can maneuver around it ok and try to go through tutorials as much as possible but some just don't show what I really need to create.
Depending on the number of layers, but if you are incrementing the rotation by say 15 degs or some number that evenly goes into 60 degrees, you will begin to repeat, so this should be fine.
I start with a hex extrusion. I started with a hex because I know I will have a nice fill pattern of hex features in a hex shape.
I then created a fill pattern. The nice thing about a fill pattern is that I can create a hex seed shape inside the feature for which will be patterned
I then created an axis about the two center planes and created a circular pattern of my hex body (a body pattern is important here)
I then just moved each body up some amount in what happens to be my y axis. This can be equation driven so you could have the moves be updated as necessary. This is the part that I just did manually as you will only have so many layers before you repeat, at which time you can do a linear pattern of your repeating bodies. However, the variable pattern in 2015 should allow you to pattern both linearly and circularly (is that a word ?) at the same time so a corkscrew patter. I don't have 2015 yet so I can't play with that...
Then I just cut to a square (remember to flip the side of cut)
This is a quick process and you are able to change you angles, overall size, etc.
This is just one possibility though so others will have good ideas as well (not that this is a good way to do it )
If you want the part, I can post it.
I also just realized you want to shift the pattern in x&y too. That could be accomplished when you do the body-move/copy command too.
This would be a good time for someone with 2015 to chime in with a variable pattern
The information is very helpful and yes could you post it and would I be able to make edits to it or changes to it?
Now after you do the cut it either to a square or circle what would be the best way to put some type of rings on the outside of the edges so everything is connected. Kind of like this image.
Here is the part.
Again, I think the variable pattern in 2015 functionality will ease the burden here.....
The rings are much easier than the hex patterns. You will use swept protrusions based upon a circle that encompasses your outer edges and then pattern that body. Let's get you to where you are happy with your hex pattern and then you can address that.
I made this one. It is a sketch of a hex, spread out using a linear sketch pattern. I made an extrude cut through a square. I then copied the sketch and edited and moved the sketch. I then created another square using the from, offset. Then i did the same with the new sketch, extrude cutting it from the offset. I dont think i had the spacing right between the two layers. I see others already added some, but since I spent the time trying it, I uploaded mine as well.
After looking at the design the only thing that I see is that I can see all the way through the design from the center and I need to not be able to see through it very well as it will look similar to a filter to strain water for instance. So more like the image that I had posted earlier.
That looks exactly as to what I am trying to design and accomplish. Any chance you could provide some more details on how you created the design? I am a beginner to SolidWorks.
Hmm, I'll try if I can. I am right in the middle of setting up a job for some parts that really need to get finished. For now, download the file and look at the sketches and extrudes and extrude cuts. I tried to make it with as few steps as i could. In a new sketch, I drew 1 hex, the size i wanted. Then I did a linear sketch pattern, with 30 degs in the x direction and 0 in the y. My hex was .500, so I chose to move .5625 in each direction. I just added enough instances to fill the area of the rectangle. I then copied the sketch and pasted it. If you have never done this, You ctrl-c while the sketch is selected, then click the plane in the tree you want it on and paste it ctrl-v. It will create another sketch. I then edited that sketch, move entities, and moved it a amount to make it offset from the first.
I made a new rectangle extrude for each layer, but I used only the original rectangle sketch. If you right click a sketch under the boss extrude, and click show, you can then click on that sketch and made another extrude. Play around with the file and see if it makes sense.
This is the offset area. You can use an existing sketch, and extrude it starting a set distance from where the sketch was created.
Great thank you and I will play around with the file you sent me. How do I get each layer to be on top of each other without really overlapping each other?
Look at cut-extrude 3
The FROM box has "offset" selected.
This will cut starting at the distance specifed. You then use a blind distance for the cut. I used .125 from each layer thickness.
Is this what you mean?
I would make 1 unit that you want, linear pattern it along a line which puts it offset 50% to the other row, and then do a linear pattern of those 2 combined units in x and y. Should allow you to create an arbitrarily large pattern exactly representing what you are seeking to do. You can do the same thing in the Z direction. Building up from individual, known correct units makes the part/assembly more editable/changable in the future if you seek to make changes, as well as making the part more stable.
Each boss extrude will be created the same way, starting at an offset from the last, or you can also select the face of the last layer as you starting point.
Here is another approach. I created a sketch that used construction lines as well to create the "nest" for which I would be using for the next layer to make sure it was aligned. The spacing then is called out as a global variable in an equation (Tools->equations).
Then the fill pattern is created, but the spacing of the fill pattern is = to the spacing variable.
Then I create another layer and create a cut that is in the center of my previously sketched honeycomb. This is only for 2 layers though. How many layers would you have as a max?
You can go in to this and change Sketch 8 and then all of the rest of the part will update.
I would need as many layers to get the overall dimensions to be 3" x 1" in size. I would want the cell size to be 22mm and the thickness to be 1.5mm.
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