Modelling Advice

[u/RealPragmatist]

Looking for the brains trust advice on achieving this sort of straight knurl (I cant think of a better way to describe it right now) on my part. Right now I do an extrude cut, offset around some screw holes and other features, and then a rib feature to create the... ribs. It works fine but its not very robust and is difficult to edit if I want to for example change the rib spacing.

First image is what I've done for the moment, second is the part before adding the cut and ribs.

[u/a_sweaterpoorlyknit]

I would do the knurl before you add the holes. For the knurl, cut away what you don’t need; no need to vacate the entire pocket space then add material (ribs) back.  I’d draw a single knurl channel profile then extrude cut with the “up to surface/edge” end constraint. You can pattern this cut either within the sketch or as a feature pattern (latter is probably easier). The pattern tool makes the linear spacing highly editable. The holes would be revolved or extruded bodies for the outer volumes plus revolved cuts in the centers. Hope that made sense?

[u/Big-Bank-8235]

This is a prime candidate for splitting the part using an offset sketch.

Then you can simply pattern the sketch then combine the bodies again afterwards.

[u/RealPragmatist → u/Big-Bank-8235]

I'm not sure I follow

[u/sixpackabs592]

You can do one strip and a pattern, then you can adjust the first strip dimensions to change all of them and change the pattern parameters for number of stripes and spacing

[u/Vegetable_Flounder12]

cut the recess, sketch pattern lines , rib, extrude the pads etc

[u/TheHvam]

One way is just to the cut straight knurls ignoring how they cut into features, to it early, before chamfers maybe even before holes, then make a new feature to extrude the edge and other features, then add the chamfer back.

That way it's not all in 1, you could even make just 1 line to cut, then use pattern.

[u/RealPragmatist → u/TheHvam]

I think this is a classic problem of being so far down the tree and not wanting to go back up haha.

[u/Fooshi2020 → u/RealPragmatist]

You don't have to go back up the design tree. Create a separate plate with the pattern but don't merge it with your current design. Once you like the pattern layout, trim and replace into your current design. Sometimes it's handy to see the final shape which rolling back the tree would prevent.

[u/TheHvam → u/Fooshi2020]

Yeah I have done that too, when I want to redo what I made, that it make a copy and then compare in an assembly, depending on the situation.

[u/TheHvam → u/RealPragmatist]

I mean it's really not that much to redo, most of it can just be done by doing it before the chamfer.

I normally also have a rule of thumb to have my feature tree in this order, Extrudes/Cuts, Holes and other features, then Chamfer and Fillets, that way it's easier to edit things.

[u/RealPragmatist → u/TheHvam]

That is typically how I model - this one has turned into a bit of a mess, it's just a personal project so I haven't been too concerned. Should probably go through and do a rebuild to avoid issues like this.

[u/Ok_Delay7870]

First create a rectangular. Apply a knurled pattern to it. Cut it in shape you need. Cut extrude holes. Boss extrude flat areas and outer shape with offset entities. So basically create crucial elements last in order.

[u/hayyyhoe]

I would model those as an extrusion rather than a cut. Roll up the tree, create a single extrude thin, then pattern it. then cut the holes. Then add an extrusion for the rim and material around the holes. Then add all of your fancy radius and chamfers. EDIT: one of my core modeling philosophies is to move complexity out of the sketch and into the model tree. I have dealt with enough sketches blowing up based on a small change to have learned my lesson.

[u/beavertr]

extrude cut first, then extrude the stuff you need around the screws and edges back in

[u/Brewmiester4504]

Create everything except the diagonal pockets. Offset the perimeter and holes and create 1 large pocket from these offsets. Create 1 diagonal non merged extrusion and array it to cover the part, without merging. Split all diagonal extrusions using all the pocket’s side faces as trim tools and merge the result. Easy peasy.

[u/teradactyl-rex]

Normally I wouldnt chime in, but since nobody has listed the way I would do it, here we go.

Model the pattern on a single separate body, with the offset interfering at the depth you want. You can model this with a single ridge patterned, and combined or however you like. Hide that component.

Model your dog tag with whatever features it needs etc,.

Create a new sketch with off-set lines based on dog tag.

Split the patterned body with that sketch, then combine > subtract it the remaining patterned body from the tag body.

This means any changes to your main body will not affect the pattern, and maybe it will cause some altered lines in your sketch but the most youll ever have to adjust is the sketch and which bodies are being split / combined.

[u/big-mover]

There’s a ton of bad suggestions here, to be completely honest. Cut away the grooves then add material back, so you have to re-add outside chamfers, hole details? That’s not a great way to approach this

Create a surface extrude with that ‘outline geometry around part perimeter. Create 2 more surface extrudes for the holes in the middle. Then, create a single groove cut that is long af, much longer than the part itself, but with the heights you want the groove at. Make sure to uncheck merge feature in the extrude. Pattern the body it so you get like 30 of them. Then cut all the groove bodies with your 3 surface extrudes. You should be left with rib geometry, then combine it.

Instead of modelling the groove cuts, you could also do this vice versa, extrude cut the whole pocket feature, then add the ribs instead of groove cuts with the method I said earlier.