Circular Pattern of a Feature & Merge???

christopher_owens

Hello!  I created a 'Revolve-Solid-Add' (a "rib" for a domed feature) and then I wanted to create a "Circular Pattern" (8 instances) of that "rib". But, the "Add" solid merged with 'Part 1' and I could not pick it or 'Revolve 2' from the Features list to revolve & copy the rib!!! Sooo, I went back to the 'Revolve 2' and changed it from 'Add' to 'New' which made it 'Part 3'. Ok, so now I can make a 'Circular Pattern' of 'Part 3' with 8 instances which created 'Part 4' to 'Part 10'!! There is no 'Merge All Instances' with a 'Merge with All' or 'Merge Scope' selection. I figure I will have to create a 'Boolean'-'Union' to merge all together.

erwin_1

Check the 'Face pattern' checkbox in the Circular pattern information window.
Then you can select al the faces of the rib to rotate.

Did a simple version here:
https://cad.onshape.com/documents/fe5099b8c2954423aa2a9d63/w/2b05d4fb23c24b6b887974c0

jakeramsley

christopher_owens said:

@andrew_troup  & @lougalloI noticed today doing a Circular Pattern-Add of a Part, that when the Part intersected itself, the parts Merged into one without selecting a Scope! Was this here before??? If the parts do not intersect (4 copies) the error is "Boolean failed...".

We treat the original part that is being patterned as part of the tools.  This lets the original part be added/removed from an external part rather than being everything except the original part. This is a by-product of that.

christopher_owens

Here is an image of what I am working on... ( I notice you can't attach a file/image while asking a question!)

christopher_owens

I may want to ultimately 3D Print this replica so it would have to be all one Boolean 'Part X' anyway for the STL file. 

erwin_1

Check the 'Face pattern' checkbox in the Circular pattern information window.
Then you can select al the faces of the rib to rotate.

Did a simple version here:
https://cad.onshape.com/documents/fe5099b8c2954423aa2a9d63/w/2b05d4fb23c24b6b887974c0

andrew_troup

Boolean union (per the OP) would also be a perfectly respectable option, and should work fine for simple geometry.

One thing to avoid in the more general case when exploring this workflow is any locale where two bodies touch only at a single edge, meaning the united body would be infinitely thin at that point. Solid modellers do not generally cope with "zero thickness geometry" like this.

Sometimes in such cases you have to use a 'thicken', towards the other body, before invoking a boolean union, if dealing with geometry which is not defined by graphic primitives like arcs and lines. If it is based on splines, there will need to be computational approximations, resulting in inevitable mismatches between nominally mating faces.

christopher_owens

Thanks Andrew! I may have to thicken the ribs into the dome feature. I also thought that I could copy using 'Duplicate' the entire 'Parts Studio 1' to a new one and create the Boolean-Merge there and create the STL from that 'Part 1'. (Did that...) Seems everything merged fine! I see as you pick parts from the Parts list they are merged and removed from that list instantly! I deleted the Boolean to try a "pick Part 1 - Shift - pick Part 10", and OS highlighted all parts in between. (Like a file manager). Also retried the Boolean dragging a window around all the displayed parts and that selected all too! Again, since I may 3D Print this project the 'Duplicate' ; 'Boolean-Merge' (for now) seems to be the way to go, as I can can now 'Transform' the Boolean Part 1 if I need to reorient it in OS for 3D Printing.

christopher_owens

Just out of curiosity, I did a  'Hide Part 2' and tried the selection methods again. Doing the "pick Part 1 - Shift - pick Part 10" selected 'Part 2', but drawing a window around the model did not pick 'Part 2' that is hidden. Ah, I see you can 'Suppress' a 'Feature', but can't 'Suppress' a 'Part X'. Wondering if the part was suppressed in the the 'Parts List' if the Shift method would select it. Yes, OS 101, but I like to see what works!!

christopher_owens

Erwin: I made my own copy of your 'Circular Pattern Test' so I could see how it was created and try something. I thought "What if I added a feature to the original solid?" So I added a 'Fillet' to the original solid. The fillet did not show up in the pattern. Ah, so I 'Reordered' the 'Fillet' before the 'Circular Pattern'. As I did this the 'Circular Pattern' failed! Hmm? OH! I needed to modify the 'Circular Pattern' to include the 'Fillet' face. Then the 'Circular Pattern' regenerated. I tried the same thing on my model where the circular pattern created new parts. I put a fillet on the original part. It did not show up on the patterned parts. I reordered the 'Fillet' before the 'Circular Pattern' and now it shows up on all the patterned parts.

christopher_owens

I had another opportunity to have Merge as an option under Circular Pattern and Mirror. Sure I can Boolean all these parts into one and will. (I am attempting to model a vase that has this pattern in it!). Just would save figuring out what Parts are what!

christopher_owens

Close! but no Shell! Actually I didn't use the above part...but it did get me thinking!

christopher_owens

Much better! Roll back, Shell, change the sketch area of the sweep from a circle to a triangle (did that in a test file first to see what effect that would have) and wa-la!

christopher_owens

One more of the Vase! Now I just need to figure out how best to make use of this!

christopher_owens

@andrew_troup  & @lougalloI noticed today doing a Circular Pattern-Add of a Part, that when the Part intersected itself, the parts Merged into one without selecting a Scope! Was this here before??? If the parts do not intersect (4 copies) the error is "Boolean failed...".

Test/recreate file image:



File that I noticed this: (Actually the Merge is what I ultimately wanted!)

jakeramsley

christopher_owens said:

@andrew_troup  & @lougalloI noticed today doing a Circular Pattern-Add of a Part, that when the Part intersected itself, the parts Merged into one without selecting a Scope! Was this here before??? If the parts do not intersect (4 copies) the error is "Boolean failed...".

We treat the original part that is being patterned as part of the tools.  This lets the original part be added/removed from an external part rather than being everything except the original part. This is a by-product of that.

shanshan

jakeramsley I also want to know when we click "add" not "new" in the circle pattern dialog window,if the parts do not intersect ,the error is "Boolean failed.." but why does not "circle pattern" show red in the feature list? Actually they are not added together,right?

Narayan_K

@christopher_owens, Boolean operation for mirror and patterns are new Improvements in onshape on 17 July.
 If the parts do not intersect for "Add" then it shows error but still the operation is performed by forming new parts in the part list.It is not only happening for mirror or pattern,we can also find the same problem while extruding also.if we define a part for "merge with" while extrude operation and the part do not intersect with extrude then also the same case....

jakeramsley

shanshan said:

jakeramsley I also want to know when we click "add" not "new" in the circle pattern dialog window,if the parts do not intersect ,the error is "Boolean failed.." but why does not "circle pattern" show red in the feature list? Actually they are not added together,right?

This behaves the same way that extrude does when you have it set to Add but doesn't touch the target.  The idea behind this is that it is a warning that the boolean failed, but that the user was making a pattern for some reason, the pattern parts succeeded, so we don't error out the feature.  The main case that we were considering with this behavior is if a user creates the pattern and changes the seed part up stream that this should have a bunch of errors when essentially it behaved as it was told to.

christopher_owens

Great update! Figured I missed the "announcement"!

christopher_owens

Just as an "I am getting the hang of this"... here is a "base plate" I will use for a "tray" that will be 3D Printed. Sketch a circle, extrude a surface, thicken, and linear pattern that now merges all into one part! Sort of an "Eureka" moment! (Actually I was trying to "lighten" the solid part by either making cuts or Boolean out a part that had a pattern. Then I noticed what I was using for the tool was actually close to what I wanted to end up with!) I have gone  back and looked at the shared "coffee cup lid", now that I know more of what I am looking at, and stepped through it's creation.  I see the "power" of all the features in Onshape. I just had to keep using them and "Unlearn what I have learned"!!  Cheers! (Now I want to recreate all my projects!) @jakeramsley @andrew_troup  @lougallo @3dcad

christopher_owens

Surface, Thicken and Linear Pattern have made this easy!

3dcad

Surface + thicken <> Extrude?

christopher_owens

Well, with the Surface + Thicken only one entity in the sketch is needed or one profile like the "wall" of the tray. Then the "wall" thickness is controlled by the Thicken. Seems the more complex the profile a Thicken would be easier. @3dcad

christopher_owens

@3dcad Example: Another part I wanted to recreate. Sketch one Spline; Extrude Surface; Thicken (which saves an Offset Sketch Entities a distance, and connecting the ends with lines.); Circular Pattern-Merge ; inner and outer rings are the two circles in the sketch Extrude and Thicken Add.

3dcad

@christopher_owens  Thanks for detailed clarification. You have interesting parts indeed.

christopher_owens

@3dcad  Well, I am creating these for a GrabCAD contest for 3D Printed accessories for a drone. I was interested in the "...used to deliver concessions in stadiums" application. I imagine beer, hot dogs, popcorn and pizza! So the parts need to be lightweight (hollow?) and with some visual "flare"! Thanks! (This is where a material density to figure part weight would be VERY handy!!!)

christopher_owens

@3dcad I just noticed using a RMB on a Part that Material can now be assigned!!

christopher_owens

Just make sure the units are set to what you want!