Circular pattern (Face option)

lucymarie_mantese

I am trying to replicate a hole around the face of my part.  The hole was generated using an extruded cut.  Based on other suggestions in the forum, I'm using the "Face Pattern" option of the "Circular Pattern" feature.  The hole is not replicating.  I would appreciate help in understanding what I'm doing wrong.  I have attached an image of the part.  The Faces to Pattern (the hole) and Axis of Pattern (the circular edge) are highlighted. Thank you.

Narayan_K

@ lucymarie_mantese, Please select end flat face hole also.Now you selected only curved face.

lucymarie_mantese

@Narayan_K, thank you for your message.  When I highlight the hole that I want to replicate, I am unable to select the flat face of the hole even when I orient the part so I am looking directly down the hole.  Is there a problem with how I generated the hole?  I attached another image zoomed in on the hole and what is highlighted as I click around the area to highlight the feature to replicate.

andrew_troup

You will need to make the model public and post the URL if you want specific guidance; it's not realistically likely we'll guess what's wrong based only on screenshots

There are lots of possible guesses, ranging from a browser problem (to fix this, hold Shift and choose "Reload" for the tab)
through modelling issues (maybe the hole is not a proper hole, but an extruded surface) through selection issues (you may have a plane showing which is above the bottom of the hole, preventing your mouse from "seeing" it), to mention a few at random.

lucymarie_mantese

@Narayan_K, I was able to resolve the issue.  After I deleted my extruded cut and re-generated it I was then able to replicate the hole. Thanks.

Narayan_K

@ lucymarie_mantese , It doesn't matter how you created hole(extrude or by hole command). Only thing is you have to select all face formed while creating hole to face pattern it.In your case the faces you selected for pattern is only one.but face formed while Extrude7 are two so you have select two faces.in simple you have specify the how depth your hole is by selecting end face.
If you are not able to select it,then please make your document public and share the link here so that we can look into that.

philip_thomas

Wow - awesome help from everyone here!
Here is my $0.02 prognostication. 
Yes you need to select both faces. 
There was nothing wrong with any of the steps you took. There is a nuance of Onshape that once internalized becomes second nature but until you have done so will frustrate you. 
Do this; extrude a square to make a block. 
Start a new sketch on the top of the block.
Draw a circle and extrude/remove downwards (recreating your hole). 
The sketch you used was automatically hidden. 
Show (un-hide) the sketch. 
Now try to select the bottom of the hole - you cannot. 
Hide the sketch. 
Now you can select the face at the bottom of the hole.
Now that you have gone through this exercise, you will never be frustrated by it again



Nerdy discussion - not necessary to read this bit! 

Why is this?
The smart Ph.D. types that write the code here tell me that because our sketches define regions (instead of the traditional concept of edges and loops), the act of creating a sketch defines a 'sheet'. The sheet covers the face on which you created the sketch. The sheet is one region and the circle you drew defines another region inside the one bounded by the face of the block. You can actually see the sheet by hiding the block. Clicking on the sheet (which is on top of the block) selects the sheet and not the block (or hole). Hiding the sketch (sheet) allows you to pick the faces underneath it. 

Quick Tip - anytime you are struggling to pick a face, you can always RMB over any sketch entity and select 'hide all sketches' - that usually does the trick. 

Feel smarter?

Narayan_K

@ philip_thomas, making sketch "Unhide", will not allow us to select face directly.But it will allow us to select face while we are in face pattern mode even if the sketch is in Un-hide condition.

 

viru

@lucymarie_mantese , Kindly refer below video which may be helpful to you.

andrew_troup

philip_thomas said:

 <large snip>

..... the act of creating a sketch defines a 'sheet'. The sheet covers the face on which you created the sketch..............

@philip_thomas 
Is the sheet bounded, and if so, by what? (particularly in the case of an open sketch, for extruding or revolving a surface)?

lucymarie_mantese

Thank you for all the comments, I appreciate the feedback.  I was able to replicate the hole that I needed for my part. 
I understood that I needed to select all faces of the hole (bottom face and curvature) but the hole I generated wasn't allowing me to do that.  Based on @philip_thomas comment, I had a hidden sketch issue. Thanks again. 

philip_thomas

@andrew_troup - here is the skinny. A sheet is infinite. If you start a sketch on a face, we 'copy' all the existing regions into the sheet. If you start a sketch on a plane, there are no regions and you just have a blank infinite sheet. There are some very cool tricks you can do with sheets. Create two concentric circles, one on each of two parallel planes. Now try to loft between them with the end conditions set to tangent. The loft fails because Onshape cannot answer the question 'tangent to what'. Now go back to each sketch and draw a box around each circle and edit the loft and re-pick the edges. Now it works because there are now two (bounded) regions (one in each sketch) that the loft can be tangent to. Yes a Phd had to show me

andrew_troup

@philip_thomas
I knew the answer would be 'interesting', but that's INTERESTING. Thanks!

ON EDIT You didn't directly address my question about open sketches [eg a conjoined pair of lines on a plane], but I think I can infer that the sheet would remain unbounded?

3dcad

@lucymarie_mantese
According to my experience using face pattern I would say it is more robust solution to do the pattern in sketch mode and add hole to each instance or extrude whole sketch (with circles).

nav

Hi @lucymarie_mantese while there is no feature based patterns https://forum.onshape.com/discussion/1050/feature-pattern I always use boolean operations or the remove option in the pattern menu. Its more reliable than face selection.