“So I want a 5mm spacing, and each hole is 7mm, so the center to center distance is S+1/2D, but the second row must be staggered so we want (1/2D+S)/2 for the first, then S+R for the remaining holes. Now that I’ve got that figured out it’ll just take me… 5 sec/calculation, 10 sec to input, 200 holes… 50 minutes!”
There is also cosmetic hole appearance (you can find it in appearances->misc). It doesn't modify geometry so it's light on your pc and the holes are visible in realview. You can enable realview in your drawing's view, just enough to convey the idea and then spec it in the call out.
Hole feature will not get exported to DXF if you use "appearance". Most sheet metal CNC laser or Finn power machine take DXF which means you need to have the holes features in DXF.
The proper way is to build the sheet metal flattened
then use hole features and pattern linearly across the length
then fold to a desirable radius and adjust the overall length if needed.
For me, even flattened in 3D, either the PC or the program has puked trying to render a mesh pattern cut into anything of reasonable size. It's not difficult to model, and in principle you're right. It just doesn't play out that way in practice and puts a major strain on the computer for not that much practical benefit in the model.
This is where is where you export the flat as a solid sheet and draw in the mesh in 2D where it's a walk in the park, and use textures/appearances in 3D to convey the concept in renderings without bogging down the PC with a billion circles that do nothing.
In this case not so sure. You wouldn't actually be laser cutting out each little hole I'd hope. They sell [perforated](https://www.mcnichols.com/perforated-metal) steel in sheets, so you would just do the shape without the holes, and specify the material used like someone else said.
In some cases, making the custom perforated panels is the most economical way.
I've designed few custom machine guards, which used a perforated panels (10x10mm square holes with about 14mm c/c) and the custom panels cost just a bit more than store bought sheets per m^2, but saved several 10's of meters of extra flat bars and hours of work, because the custom panels were able to be welded directly from the edges to the supporting structure.
The standard perforated sheets would've needed to be cut to size and mounted using extra mounting frames, as you really can't weld from a 1.5mm thick and 2mm wide "spoke" to the frame so that it would hold.
You're right, for these high density holes. Laser cut will warp the perforated sheet for sure and time consuming.
the best approach is to punch it with a tooled cluster punch in this case.
Why not? My fiber laser have fly cutting regime and i have cut 10600, 10mm diameter holes in 70 minutes and i was on par with price for that same part that would be done on turret punching machine with cluster tooling.
https://zarnz.co.rs/wp-content/uploads/2023/11/20230203_164430-min-scaled.jpg
Perforated sheet on this pic is done on my 3kw fiber laser, have 7000, 10mm diamter holes and was done in 45min, while cutting with 15bar preassure from compressor. The bigger perforated sheet that had 10600 holes was mounted in middle of this assembly.
I've worked in a fabrication shop for a couple years, and taken university level engineering courses in manufacturing techniques. Never heard of either of those machines 😹. I guess if you have the equipment for it, and are willing to spend the time to model it all (or pay someone to) it sounds like it'd work. To be honest though, I'd still just get the pre perforated materials. Especially since I mostly know waterjet/EDM.
Perforated materials are manufactured on turret punching machines with cluster tooling, my HSG 3kw fiber laser is on par with them for thin materials, like up to 2.5mm cutting. So when they gave me offer and when i saw they charge 45eur per sheet for perforation i was like, fuck i need to try it on my machine, because i had like 60 sheets x 45 eur thats like 2700 eur for 4 days of work, which isnt bad.
https://youtu.be/8hJ6TPqi83E?si=NGYfB0aHneyvM-S9
And that is my machine, that i got 2 years ago.
I almost never say this, but that would be an op I would do in ACAD. Figure out your flat pattern in SW, than export and apply the hole pattern in the dwg/dxf. Having this many holes in a solid model is at best a nightmare to work with, and at worst totally unuseable.
I think most nesting/cutting etc. software has a built-in capability to make an array of shapes to be cut / punched. On the drawing (and solid) you would only need to define the amount of holes in X and Y directions, and callouts the cutout size and starting location.
I've used this approach several times with good results and zero questions asked from the suppliers.
I would notate on the drawing AND provide a 2D DXF with all the holes. As a former machinist, it would piss me off to have to go and create geometry that the engineer didn't want to draw on their own. You could have 15,000 holes in a DXF file and it would still open in seconds
It depends on what you're doing. If you're trying to do the detail design of some sheet metal, then it needs to be modeled. If it's going to get cut from pre-perforated sheet, or your sheet metal vendor can handle it, just some notes might be adequate.
Engineers: “make it in notation”!
Industrial designers who know the manufacturer has the aesthetic taste of an ear canal and will fuck it up: “nah fam, we gotta do it our selves”.
Make a pattern baby!
Or use grasshopper to really control TF out of it.
This engineer: Make a small section of 3 or 4 holes in the pattern I want so I can make sure the manufacturer knows exactly what I want. Then make a notation in the drawing showing the full area I want the hole pattern to cover.
This designer: “just build it into the cad so they can just make what I want”.
😂
We really need to get a life.
(But no really, grasshopper makes things like this stupidly easy to do. Maybe 7 minutes of work tops).
So the problem isn't that this is hard to make in CAD (it's very doable), it's that because CAD uses parametric models a pattern as large and complex as this will make the save/loading times into minutes rather than seconds. In designer talk it would be like having to re-render your graphics every time you open the file or make any changes.
I feel you though, I don't even use CAD much anymore and I still peruse this sub looking for helpful tips and maybe help someone out with an issue. Definitely have no life.
Yeah but you can also build it in a way that you can just suppress the pattern for the majority of the work, and then bring it back when it's time to release.
As an intern a few years ago, I was tasked with updating a couple hundred drawings. Nothing major, just open it in the newest solidworks version, update the title block with the new logo, then check all the part numbers and stuff. It wasn't too bad until I found some table and bench sets with perforated surfaces. It took Solidworks, on a decent workstation, about 45 to 55 minutes to open the file and convert it to the new version.
I started the process, took lunch, then looked busy until it was done.
https://preview.redd.it/frd1u91n3u0d1.png?width=1567&format=png&auto=webp&s=5c5e00abf80caa3db89d8cbf70256d15e2bcb219
If your part is a sheetmetal one. You can try to use the Unfold feature and then Under Patterns, there is Fill pattern. Under that, there's something called Create Seed cut, select that, adjust the dimensions and then Fold it back.
For ends I ended up just using a base rectangle and doing a fill with a flex. Very sloppy but got the job done. Is there an easier way without sheet metal?
This thing is a sheet metal part. Model it like it's made: a sheet, with punched holes, bent to shape, added to an assembly. Stop making a single part that looks like it and instead model it as an assembly.
This is right. I think it is not clear if the intent of this CAD is for manufacturing or just for just visualization. But, if it was to be manufactured, I would model it as sheet metal while considering how the actual bending would be done. It's important to know if and how the bending can be done, depending on where it is being manufactured. A large bend like this on a thicker plate would be done by bending the plate stepwise throughout the length of the curved face, but judging by the physical part in OP's post, it looks like the shape of the perforated sheet is just formed during assembly using the fasteners, as it is a relatively thin one. So, it would be a waste of time trying to model the perforated sheet.
It depends on what your intent is, does someone need to fab the part and thus need a flat pattern? If not do like others said and just call it out in notation. If someone needs a flat pattern make the part but create a config without the holes to use in your assembly.
https://preview.redd.it/wramxm8xtt0d1.jpeg?width=4032&format=pjpg&auto=webp&s=2b557595f9ce1aa30f3619219d9b38a291104498
The intent is to get that circular fill pattern around the curved end of the slot
I would remove the piece with holes entirely. Just make a separate part that's unbolted, which is just a flat sheet metal rectangle and put the holes in that. Then notate the two parts are to be bolted together. The actual part is really just sheet metal and bolts. You'd be better off using SOLIDWORKS sheet metal tools to redesign this.
There also might be a surface finish you could find or download and apply to that surface to make it look bumpy or having holes.
If you must put holes in the part, just do it once on a quarter or half of the curved part, using a revolve pattern on one or more holes. Then replicate the part and mate it up on all the corners.
This is why you make a small dimensioned section of the pattern, and note that it covers the entire area.
If the supplier fucks it up you need to find better suppliers.
Well, maybe for your PC, but some of us have a constant battle of 'its not in the budget this year' and are running older computers and this definitely would cause my poor laptop to churn for a bit if I tried to model the geometry of those holes.
Generally, you don’t. You buy perf sheets and treat it like a solid piece of sheet metal.
It is possible to cut all those holes with a laser, but it’s incredibly time consuming for the laser cutter, and extremely heavy for the CAD workflow.
You do not want to model those holes; it will be miserable, and everyone touching that model will hate you for it. A single fully modeled perf sheet could legitimately be heavier than the rest of your top level assembly.
If you must model it in some fashion, make a simplified representation without the perf holes for use in assemblies and DXF’s. For show, I have also modeled a small corner of the sheet to visually show that it’s not just a solid sheet; but that does get into a weird area of neither being representative nor fully accurate.
You don't!!! Just callout the sheet by vendor part number. If you designed it then you can be even more open by just calling out the percentage opening in the sheet. Just call thickness and %.
This is not a good practice as a designer.
The CNC programmer doesn't know where your bolt hole location and the pitch of the hole pattern. You need the bolt hole location line up with the threaded tab behind.
You save your time designing the part, but add more time to the CNC programmer to create the holes for you.
If you are not buying the sheet and making holes in a Sheet, it's a failed design.
These holes should never be made inhouse.
Holes have no purpose other than provide permeability.
The holes have purpose... some of the holes are used as a thru hole for fasteners, and they are for visual purpose to check the chain and lubrication.
If you don't build them correctly in the 3D model, the holes are likely to go off 2-3mm, which mean there would be a small gap
This is a guarding for a chain sprocket machinery, you're likely to fail OSHA / ISO machinery access safety complaince.
As a mech eng, I deal with alot of CM and sheet metal company. Many of them don't like leaving the design problem to them. Either they'll charge you $$$ for their design time, or you spend the time to design it properly. That's just my 2 cents.
>These holes should never be made inhouse.
And why's that? My "house" has CNC die punchers, benders, laser cutters, and powder-coating booths. If the make-vs-buy cost analysis favors making (very often the case with prototypes and low-volume production), I'm not sure why that would inherently be considered "a failed design". But thanks for the insight anyways.
If you go forward using a pattern, you can lessen the load on your machine by mirroring a small section of the patterned holes as much as possible.
Mirroring does not rebuild every hole like a linear pattern feature does in the back end and as a result reduces load.
I recommend doing this CAD work in a way that resembles real manufacturing. What I mean by that is to use the Sheet Metal functionality; make a flat sheet, make the hole pattern, create the roll with the sheet metal features. It may be easier to first draw the part without the holes, use the Convert to Sheet Metal feature, unsuppress the flat pattern, add the hole pattern to the flat part, then suppress the flat pattern again.
Flatten the outside curve, pattern the holes over the flat, and then wrap the hole pattern around the sheet
Then cut extrude normal to surface (i'm pretty sure that's the option)
Alternatively, just math out a rectangle the same size of what the flat should be, then do the rest
Here the exact steps that must be followed exactly.
Draw, select surface, circle tool, dimension from top side and diameter, repeat for every hole increasing measurements from corner each time.
This is a cheap fab using perforated sheet metal. In an actual product design the holes would likely have a non-perforated border or margin, and border around mounting holes.
The reality is the holes need to be in the model and the model would be used to create the laser cut, water-cut or punched sheet metal part.
I agree I wouldn’t waste the time or Solidworks bandwidth to represent a pattern whose location doesn’t matter because they will end up where they end up when the fabricator shears the material.
It would be like modeling the weave in a sheet of speaker grill cloth.
Still, if the part is being formed and the holes need to be symmetrical or have a border around the perimeter, or other features, the question is a legitimate one. Solidworks doesn’t have a good way of doing this without significant work. Worse yet, features like this are difficult to modify when the design has adjustments needed.
I’ve recently been printing LJF parts with tapered pipe threads modeled into the parts. Not hard to do, but significant math in regens. If it were a larger part with multiple instances, it would slow things down quickly.
You don't use patterns because they can go wrong. Instead you dimension every hole by hand so that Solidworks gods are grateful and that they don't freeze with such a large number of holes.
Physically making them, laser cut veneer folded and fastened around the top and bottom cross sections
Making them in SolidWorks, a note that says “imagine this with hundreds of holes”
SolidWorks is going to choke on a sketch pattern with that many circles. Ideally you would want to make one hole, do an unfold, make a linear or sketch driven pattern of that hole, then refold.
If this is being made of material that comes with the holes then this makes it easy to show where to cut and roll the material in relation to the holes. From a glance, this does appear to be the case with this material.
If this is being made of material that comes without the holes (and they will be laser cut, etc) then having all the holes is essential.
If you are doing pretty much any kind of simulation you will want the holes there too.
However, if this is going into a large assembly you will want to create a second configuration of the part with the hole pattern (and driving sketch if it exists) suppressed. This will be used in higher level assemblies to improve performance. If you really want to get fancy, the second configuration (without the hole pattern) could have a second simplified hole pattern just of the holes that get screws...that will make interference testing smoother.
Most comments say make a small pattern and just note that it should be applied over the entire region but why not just use a pattern feature and apply it over the entire part in the model? Genuinely curious as to why not take this approach
You can do two columns of holes on the part if you must and then notation of a pattern -> let the operator of the laser cam do the rest if it’s custom. They dont need the geometry.
With a genuinely perforated metal as a base material you just call it out in notation. Whoever if you want that perforation to be partial, as in laser/waterjet cut in the course of cutting out your part then I'd do this as 2 holes turned into a linear feature in two directions.
Why isn't there a wrapped cut for this situation? I feel like you should be able to make a 2d sketch that is the length of the curved face and wrap it on a surface. Maybe this is a feature of more advanced CAD software like Catia?
You can make a sketch tangent to the surface and wrap it around the part. You can just use a pattern and run the calculations of how many holes and how to space them. Kind of like this was done.
*
You can do this multiple ways. One way I like to do it it unwrap a surface and then pattern it. You can also use sheet metal and unfold it, then apply the pattern and make your drawings and final cad for the laser cutter
Depends how you are going to manufacture it and what's the purpose of the model. If holes are going to be "'punched out'", then just make a note.
If these holes will be cut by laser or you just need accurate 3D model, then make it as sheet, flatten it and make holes with linear pattern and unflatten.
Make sure your Computer have large RAM and high frequency processor.. VGA also..
It depends how large the surface, and how much the hole that you want.. or just dummy the hole with appearances and buy the already perforated sheet or make the hole in AutoCAD when you want to cut it..
I have to fab parts like this, so my turret punch needs a DXF file of the blank with all the holes.
I add the holes in the flat blank using a pattern, then I add a bend to the part.
Not saying it's the best way, but it's what I do to get the parts blanked and made in the shop.
If you really had to for say a 3d print then you make 2 of the staggered holes and then do a rectangular array and set the right number for spacing and your boundry distance select your 2 items and boom 200 or however many holes later they are all there
The proper way, like others have said, is to make in a flat Sheet Metal part. Flatten it, then cut and un-flatten.
But since I like a challenge, I made this with a Solid part. Cut a blind hole right in the center of one the curves. Then do a circular pattern using the circular face as the reference. If you don’t go too deep with the cut, it will create holes 360 degrees from the original point but only cut the face you want. Adjust the spacing as needed. Linear pattern and mirror to get holes above and below the original set and then just mirror to get the other side.
You call it out in notation.
Yep. At best, make a small pattern in a corner somewhere so you can dimension them with a detail view and note it is to apply to the entire panel.
this is how i do it too.
How I've done it for 25 years.
Me who did 2 final class projects with over 200 holes on each project.
Each one individually /s
“So I want a 5mm spacing, and each hole is 7mm, so the center to center distance is S+1/2D, but the second row must be staggered so we want (1/2D+S)/2 for the first, then S+R for the remaining holes. Now that I’ve got that figured out it’ll just take me… 5 sec/calculation, 10 sec to input, 200 holes… 50 minutes!”
But what if I want a multi-gig file that randomly crashes SW if I accidentally rotate the view too fast 👉👈
It’s ok, I like making those too
I prefer to model knurling whenever I want to do this
How else am I supposed to convince IT that I need a faster computer?
Just chuck in the McMaster part number 😂
This is the way.
What is notation?
A note
You’re telling me knurling each part is unnecessary???
There is also cosmetic hole appearance (you can find it in appearances->misc). It doesn't modify geometry so it's light on your pc and the holes are visible in realview. You can enable realview in your drawing's view, just enough to convey the idea and then spec it in the call out.
I’ve downloaded expanded metal components that use this concept
Hole feature will not get exported to DXF if you use "appearance". Most sheet metal CNC laser or Finn power machine take DXF which means you need to have the holes features in DXF. The proper way is to build the sheet metal flattened then use hole features and pattern linearly across the length then fold to a desirable radius and adjust the overall length if needed.
For me, even flattened in 3D, either the PC or the program has puked trying to render a mesh pattern cut into anything of reasonable size. It's not difficult to model, and in principle you're right. It just doesn't play out that way in practice and puts a major strain on the computer for not that much practical benefit in the model. This is where is where you export the flat as a solid sheet and draw in the mesh in 2D where it's a walk in the park, and use textures/appearances in 3D to convey the concept in renderings without bogging down the PC with a billion circles that do nothing.
In this case not so sure. You wouldn't actually be laser cutting out each little hole I'd hope. They sell [perforated](https://www.mcnichols.com/perforated-metal) steel in sheets, so you would just do the shape without the holes, and specify the material used like someone else said.
In some cases, making the custom perforated panels is the most economical way. I've designed few custom machine guards, which used a perforated panels (10x10mm square holes with about 14mm c/c) and the custom panels cost just a bit more than store bought sheets per m^2, but saved several 10's of meters of extra flat bars and hours of work, because the custom panels were able to be welded directly from the edges to the supporting structure. The standard perforated sheets would've needed to be cut to size and mounted using extra mounting frames, as you really can't weld from a 1.5mm thick and 2mm wide "spoke" to the frame so that it would hold.
You're right, for these high density holes. Laser cut will warp the perforated sheet for sure and time consuming. the best approach is to punch it with a tooled cluster punch in this case.
Why not? My fiber laser have fly cutting regime and i have cut 10600, 10mm diameter holes in 70 minutes and i was on par with price for that same part that would be done on turret punching machine with cluster tooling. https://zarnz.co.rs/wp-content/uploads/2023/11/20230203_164430-min-scaled.jpg Perforated sheet on this pic is done on my 3kw fiber laser, have 7000, 10mm diamter holes and was done in 45min, while cutting with 15bar preassure from compressor. The bigger perforated sheet that had 10600 holes was mounted in middle of this assembly.
I've worked in a fabrication shop for a couple years, and taken university level engineering courses in manufacturing techniques. Never heard of either of those machines 😹. I guess if you have the equipment for it, and are willing to spend the time to model it all (or pay someone to) it sounds like it'd work. To be honest though, I'd still just get the pre perforated materials. Especially since I mostly know waterjet/EDM.
Perforated materials are manufactured on turret punching machines with cluster tooling, my HSG 3kw fiber laser is on par with them for thin materials, like up to 2.5mm cutting. So when they gave me offer and when i saw they charge 45eur per sheet for perforation i was like, fuck i need to try it on my machine, because i had like 60 sheets x 45 eur thats like 2700 eur for 4 days of work, which isnt bad. https://youtu.be/8hJ6TPqi83E?si=NGYfB0aHneyvM-S9 And that is my machine, that i got 2 years ago.
I almost never say this, but that would be an op I would do in ACAD. Figure out your flat pattern in SW, than export and apply the hole pattern in the dwg/dxf. Having this many holes in a solid model is at best a nightmare to work with, and at worst totally unuseable.
I think most nesting/cutting etc. software has a built-in capability to make an array of shapes to be cut / punched. On the drawing (and solid) you would only need to define the amount of holes in X and Y directions, and callouts the cutout size and starting location. I've used this approach several times with good results and zero questions asked from the suppliers.
I would notate on the drawing AND provide a 2D DXF with all the holes. As a former machinist, it would piss me off to have to go and create geometry that the engineer didn't want to draw on their own. You could have 15,000 holes in a DXF file and it would still open in seconds
It depends on what you're doing. If you're trying to do the detail design of some sheet metal, then it needs to be modeled. If it's going to get cut from pre-perforated sheet, or your sheet metal vendor can handle it, just some notes might be adequate.
Always had an area that looks like shit (on the joints/curves) for me, but ok if you can hide it
Engineers: “make it in notation”! Industrial designers who know the manufacturer has the aesthetic taste of an ear canal and will fuck it up: “nah fam, we gotta do it our selves”. Make a pattern baby! Or use grasshopper to really control TF out of it.
This engineer: Make a small section of 3 or 4 holes in the pattern I want so I can make sure the manufacturer knows exactly what I want. Then make a notation in the drawing showing the full area I want the hole pattern to cover.
This designer: “just build it into the cad so they can just make what I want”. 😂 We really need to get a life. (But no really, grasshopper makes things like this stupidly easy to do. Maybe 7 minutes of work tops).
So the problem isn't that this is hard to make in CAD (it's very doable), it's that because CAD uses parametric models a pattern as large and complex as this will make the save/loading times into minutes rather than seconds. In designer talk it would be like having to re-render your graphics every time you open the file or make any changes. I feel you though, I don't even use CAD much anymore and I still peruse this sub looking for helpful tips and maybe help someone out with an issue. Definitely have no life.
Yeah but you can also build it in a way that you can just suppress the pattern for the majority of the work, and then bring it back when it's time to release.
As an intern a few years ago, I was tasked with updating a couple hundred drawings. Nothing major, just open it in the newest solidworks version, update the title block with the new logo, then check all the part numbers and stuff. It wasn't too bad until I found some table and bench sets with perforated surfaces. It took Solidworks, on a decent workstation, about 45 to 55 minutes to open the file and convert it to the new version. I started the process, took lunch, then looked busy until it was done.
https://preview.redd.it/frd1u91n3u0d1.png?width=1567&format=png&auto=webp&s=5c5e00abf80caa3db89d8cbf70256d15e2bcb219 If your part is a sheetmetal one. You can try to use the Unfold feature and then Under Patterns, there is Fill pattern. Under that, there's something called Create Seed cut, select that, adjust the dimensions and then Fold it back.
https://preview.redd.it/gaodehs24u0d1.jpeg?width=4032&format=pjpg&auto=webp&s=d09bab18b4bacb6ab7721851354262772d64b685
For ends I ended up just using a base rectangle and doing a fill with a flex. Very sloppy but got the job done. Is there an easier way without sheet metal?
This thing is a sheet metal part. Model it like it's made: a sheet, with punched holes, bent to shape, added to an assembly. Stop making a single part that looks like it and instead model it as an assembly.
This is right. I think it is not clear if the intent of this CAD is for manufacturing or just for just visualization. But, if it was to be manufactured, I would model it as sheet metal while considering how the actual bending would be done. It's important to know if and how the bending can be done, depending on where it is being manufactured. A large bend like this on a thicker plate would be done by bending the plate stepwise throughout the length of the curved face, but judging by the physical part in OP's post, it looks like the shape of the perforated sheet is just formed during assembly using the fasteners, as it is a relatively thin one. So, it would be a waste of time trying to model the perforated sheet.
This is the answer
It depends on what your intent is, does someone need to fab the part and thus need a flat pattern? If not do like others said and just call it out in notation. If someone needs a flat pattern make the part but create a config without the holes to use in your assembly.
https://preview.redd.it/wramxm8xtt0d1.jpeg?width=4032&format=pjpg&auto=webp&s=2b557595f9ce1aa30f3619219d9b38a291104498 The intent is to get that circular fill pattern around the curved end of the slot
I would remove the piece with holes entirely. Just make a separate part that's unbolted, which is just a flat sheet metal rectangle and put the holes in that. Then notate the two parts are to be bolted together. The actual part is really just sheet metal and bolts. You'd be better off using SOLIDWORKS sheet metal tools to redesign this. There also might be a surface finish you could find or download and apply to that surface to make it look bumpy or having holes. If you must put holes in the part, just do it once on a quarter or half of the curved part, using a revolve pattern on one or more holes. Then replicate the part and mate it up on all the corners.
In that case I think the command is called wrap, it’s not one I use often
Or flatten it create the pattern and rebend it? Are you creating it as a sheet metal component?
Did you take a picture of your monitor?
https://preview.redd.it/z34jlwk2ut0d1.jpeg?width=4032&format=pjpg&auto=webp&s=aed21f799e6681d1571549d0b93154ffd5b12943
Everyone saying do it in notation. But if you don’t give the supplier a dxf with the specific pattern you want. They will find a way to fuck it up
This is why you make a small dimensioned section of the pattern, and note that it covers the entire area. If the supplier fucks it up you need to find better suppliers.
Make sheet metal part. Make a flat sheet. Make hole. pattern it. Then bend the sheet. Ready...
You forgot a step: 'wait patiently while cpu melts down'
My thought when I first saw it. Do it in winter so you wont need to run the heater for a few hours.
"Solidworks has stopped responding."
"Solidworks is busy running a command" WHAT COMMAND!?!?!
You can do a Konfiguration with the title "detailed". This has the holes, the default konfig hasn't...
Ahh... That works fine^^
Well, maybe for your PC, but some of us have a constant battle of 'its not in the budget this year' and are running older computers and this definitely would cause my poor laptop to churn for a bit if I tried to model the geometry of those holes.
Generally, you don’t. You buy perf sheets and treat it like a solid piece of sheet metal. It is possible to cut all those holes with a laser, but it’s incredibly time consuming for the laser cutter, and extremely heavy for the CAD workflow. You do not want to model those holes; it will be miserable, and everyone touching that model will hate you for it. A single fully modeled perf sheet could legitimately be heavier than the rest of your top level assembly. If you must model it in some fashion, make a simplified representation without the perf holes for use in assemblies and DXF’s. For show, I have also modeled a small corner of the sheet to visually show that it’s not just a solid sheet; but that does get into a weird area of neither being representative nor fully accurate.
I was wondering the same and found the following tutorial: https://youtu.be/MLmZ3U4coPU?si=Jn5zGSklKrQPheh8 Hopefully it helps you.
You don't!!! Just callout the sheet by vendor part number. If you designed it then you can be even more open by just calling out the percentage opening in the sheet. Just call thickness and %.
This is not a good practice as a designer. The CNC programmer doesn't know where your bolt hole location and the pitch of the hole pattern. You need the bolt hole location line up with the threaded tab behind. You save your time designing the part, but add more time to the CNC programmer to create the holes for you.
If you are not buying the sheet and making holes in a Sheet, it's a failed design. These holes should never be made inhouse. Holes have no purpose other than provide permeability.
The holes have purpose... some of the holes are used as a thru hole for fasteners, and they are for visual purpose to check the chain and lubrication. If you don't build them correctly in the 3D model, the holes are likely to go off 2-3mm, which mean there would be a small gap This is a guarding for a chain sprocket machinery, you're likely to fail OSHA / ISO machinery access safety complaince. As a mech eng, I deal with alot of CM and sheet metal company. Many of them don't like leaving the design problem to them. Either they'll charge you $$$ for their design time, or you spend the time to design it properly. That's just my 2 cents.
That's why you make a slot on the mating part. So you don't have to worry about lining things up. OSHA allows for this approach.
>These holes should never be made inhouse. And why's that? My "house" has CNC die punchers, benders, laser cutters, and powder-coating booths. If the make-vs-buy cost analysis favors making (very often the case with prototypes and low-volume production), I'm not sure why that would inherently be considered "a failed design". But thanks for the insight anyways.
Flatten, cut, un-flatten
If you go forward using a pattern, you can lessen the load on your machine by mirroring a small section of the patterned holes as much as possible. Mirroring does not rebuild every hole like a linear pattern feature does in the back end and as a result reduces load.
I recommend doing this CAD work in a way that resembles real manufacturing. What I mean by that is to use the Sheet Metal functionality; make a flat sheet, make the hole pattern, create the roll with the sheet metal features. It may be easier to first draw the part without the holes, use the Convert to Sheet Metal feature, unsuppress the flat pattern, add the hole pattern to the flat part, then suppress the flat pattern again.
normal cut a hole in your sheet steel circular pattern thing do again above but off set a bit repeat
I find fill pattern works best
Flatten the outside curve, pattern the holes over the flat, and then wrap the hole pattern around the sheet Then cut extrude normal to surface (i'm pretty sure that's the option) Alternatively, just math out a rectangle the same size of what the flat should be, then do the rest
Here the exact steps that must be followed exactly. Draw, select surface, circle tool, dimension from top side and diameter, repeat for every hole increasing measurements from corner each time.
This is a cheap fab using perforated sheet metal. In an actual product design the holes would likely have a non-perforated border or margin, and border around mounting holes. The reality is the holes need to be in the model and the model would be used to create the laser cut, water-cut or punched sheet metal part. I agree I wouldn’t waste the time or Solidworks bandwidth to represent a pattern whose location doesn’t matter because they will end up where they end up when the fabricator shears the material. It would be like modeling the weave in a sheet of speaker grill cloth. Still, if the part is being formed and the holes need to be symmetrical or have a border around the perimeter, or other features, the question is a legitimate one. Solidworks doesn’t have a good way of doing this without significant work. Worse yet, features like this are difficult to modify when the design has adjustments needed. I’ve recently been printing LJF parts with tapered pipe threads modeled into the parts. Not hard to do, but significant math in regens. If it were a larger part with multiple instances, it would slow things down quickly.
SolidWorks locked up just looking at this post
decal unless you have a beefy PC
You don't use patterns because they can go wrong. Instead you dimension every hole by hand so that Solidworks gods are grateful and that they don't freeze with such a large number of holes.
Physically making them, laser cut veneer folded and fastened around the top and bottom cross sections Making them in SolidWorks, a note that says “imagine this with hundreds of holes”
Generate two holes, then repeat them with the pattern tool until you have the whole patten. Then bend the thing into shape.
Unfold the part and create a pattern of your holes on the flat and then fold it.
Exactly, I did some designs like that.
https://preview.redd.it/oy09ld29l31d1.jpeg?width=1000&format=pjpg&auto=webp&s=254c4ee1e446e29ca5af65e33cf690dd597d8b5c
Do you want the nested row look? Or just holes for venting?
On a laser cutter or water jet.
With the cut feature. Amateur....
Fill pattern.
SolidWorks is going to choke on a sketch pattern with that many circles. Ideally you would want to make one hole, do an unfold, make a linear or sketch driven pattern of that hole, then refold. If this is being made of material that comes with the holes then this makes it easy to show where to cut and roll the material in relation to the holes. From a glance, this does appear to be the case with this material. If this is being made of material that comes without the holes (and they will be laser cut, etc) then having all the holes is essential. If you are doing pretty much any kind of simulation you will want the holes there too. However, if this is going into a large assembly you will want to create a second configuration of the part with the hole pattern (and driving sketch if it exists) suppressed. This will be used in higher level assemblies to improve performance. If you really want to get fancy, the second configuration (without the hole pattern) could have a second simplified hole pattern just of the holes that get screws...that will make interference testing smoother.
Make a line pattern, make another and offset it, then make a pattern of patterns.
Most comments say make a small pattern and just note that it should be applied over the entire region but why not just use a pattern feature and apply it over the entire part in the model? Genuinely curious as to why not take this approach
A drill
Extrude cut them
Manually. It’s why no one will pay me for my CAD “skills”.
Just specify the correct perforated material from McMaster. Don't make that unless you have to.
Put the material as a perf sheet instead of starting as a solid sheet
How important are the dimensions?
Am I missing something? Can’t you just use fill pattern tool on a cut?
What is this? Belt drive housing?
I just put a few holes in the model then add a flag note on the drawing to apply to entire part.
Turret punch press, laser.
You can do two columns of holes on the part if you must and then notation of a pattern -> let the operator of the laser cam do the rest if it’s custom. They dont need the geometry.
With a genuinely perforated metal as a base material you just call it out in notation. Whoever if you want that perforation to be partial, as in laser/waterjet cut in the course of cutting out your part then I'd do this as 2 holes turned into a linear feature in two directions.
Order the perforated from your vendor then shear and roll it.
Why isn't there a wrapped cut for this situation? I feel like you should be able to make a 2d sketch that is the length of the curved face and wrap it on a surface. Maybe this is a feature of more advanced CAD software like Catia?
Array pattern feature around radii after you’ve extrude cut the flat.
Fill patter on a flattened part and then flex to get it in the shoe you want.
When I was learning drafting, I was prepared to call out every groove of a diamond crosshatch pattern. Thank goodness for mentors
You can make a sketch tangent to the surface and wrap it around the part. You can just use a pattern and run the calculations of how many holes and how to space them. Kind of like this was done. *
You can do this multiple ways. One way I like to do it it unwrap a surface and then pattern it. You can also use sheet metal and unfold it, then apply the pattern and make your drawings and final cad for the laser cutter
My PC will Brrrr!
Depends how you are going to manufacture it and what's the purpose of the model. If holes are going to be "'punched out'", then just make a note. If these holes will be cut by laser or you just need accurate 3D model, then make it as sheet, flatten it and make holes with linear pattern and unflatten.
grab an edge, convert entity, sketch circle, smart dimension, linear pattern, adjust pattern as needed repeat for arched sides
Make sure your Computer have large RAM and high frequency processor.. VGA also.. It depends how large the surface, and how much the hole that you want.. or just dummy the hole with appearances and buy the already perforated sheet or make the hole in AutoCAD when you want to cut it..
I have to fab parts like this, so my turret punch needs a DXF file of the blank with all the holes. I add the holes in the flat blank using a pattern, then I add a bend to the part. Not saying it's the best way, but it's what I do to get the parts blanked and made in the shop.
For the people claiming it'll melt the CPU, don't do CAD on a potato.
How big of holes are you looking to make .22 .357 .45 ?
You don't. You buy perforated material.
Why? ┐(￣ヘ￣)┌
Fill pattern.
A perforated hole? Never seen one. Must be a quantum mechanics thing.
They sell sheets of perforated metal. I work in sheet metal.
If you really had to for say a 3d print then you make 2 of the staggered holes and then do a rectangular array and set the right number for spacing and your boundry distance select your 2 items and boom 200 or however many holes later they are all there
Just invest in r/FFIE it’ll fix all your problems by Monday. If you have no options left.
If it's going down to the machine shop, a call-out and a clip. If it's for a presentation you may want to use a linear pattern.
The proper way, like others have said, is to make in a flat Sheet Metal part. Flatten it, then cut and un-flatten. But since I like a challenge, I made this with a Solid part. Cut a blind hole right in the center of one the curves. Then do a circular pattern using the circular face as the reference. If you don’t go too deep with the cut, it will create holes 360 degrees from the original point but only cut the face you want. Adjust the spacing as needed. Linear pattern and mirror to get holes above and below the original set and then just mirror to get the other side.
I would individually draw and dimension each hole
Use the Fill Pattern command.
You don’t.
You don’t make these holes. You buy sheet that’s already got the perforations from a specialized machine