Can I make a circular pattern of sketches? 1

[amlsna]

Greetings,
I am trying to create a circular pattern with sketches, however each time I try I do not get the sketch to pattern around the circle. Basically, I have a disc, with rectangles (3) at 120 degree BC along the outer edge. I am using the sketches for the assembly to use as mate features for the parts. My question is, I can put a single rectangle that is on the outer rim of the disc, but I am not able to have that patterned around the disc. Any ideas, I am probably missing the obvious, so I am asking.
Thanks,

 

[ksudavid]

amlsna,

You cannot pattern sketch entities but you can create sketch patterns that can be used to drive assy part patterns. Create a single sketch on your disk and use it to locate the first rectangle in your assy. Now create an assy sketch that contains a 3 instance circular pattern. While creating the sketch profile you will see the circular pattern tool on your toolbar.

Exit the sketch and choose Pattern from the toolbar. Select your rectangular part and use the sketch pattern you created to drive your part pattern.

The confusing thing is distinguishing between the sketch pattern and the part pattern. In the assy you are creating a sketch pattern to drive the part pattern.

Hope this isn't too confusing. If you are running V19 I can send you an example file.

 

[amlsna]

ksudavid,
Unfortunately, we are stuck with V17 until spring time and then will have V19. I am a little confused on the sketch in the assembly. I am in the assy, and I am not sure how or what you are referring to with the 3 instance circular pattern? My steps are: (in the assembly)
1. click sketch
2. click surface that the pattern will be on
3. create rectangle at 1st known location.
4. click the circular pattern button
5. set options to fit w/ instances = 3.
6. then have to create start pt of arc, thus giving me a useless circle and no pattern / instances.

This is where I am stuck. Ideas / Clarifications.
Thanks,

 

[donyoung]

amlsna,

AFAIK you can't pattern a sketch. But what about this
approach to define the pattern along with the disc?
The rectangle can be created as Extruded surface.
Make it with closed ends and very thin the direction
of the extrusion should point into the disc so that one
surface is flush with the disc
Now this surface can be use in pattering (select Body for
the item to be included in the pattern)
When this part is inserted into the assembly activate
'Show Surfaces'. Now you can place parts and constrain
them to these surfaces like you could do with 'normal'
surfaces

Pattern

dy

 

[amlsna]

dy,
Thanks, I was trying to see if there was another way to get this done. I have done a different approach with sketches and having them driven by the first sketch and then using some associations in case I change some features, which got me the desired results. I was just hoping that someone had another trick that would be as simple as being able to pattern a sketch. I guess that will be an enhancement request for V20.
Thanks again,
amlsna

 

[amlsna]

dy,
Real quick, your file is V18 and I am on V17, so couldn't use it. thanks though.

 

[donyoung]

amlsna,

I've replace the file by a V16 one, the link above is
still valid, so it still reads ..._V18.zip

dy

 

[donyoung]

amlsna,


1. click sketch
OK
2. click surface that the pattern will be on
OK
3. create rectangle at 1st known location.
OK
4. click the circular pattern button
OK
5. set options to fit w/ instances = 3.
OK
6. then have to create start pt of arc, thus giving me a useless
circle and no pattern / instances.
OK
This circle is your Assembly pattern. If you look carefully
you will spot 3 crosses on the circle these will later
the positions for the parts to pattern

7. now leave the sketch, Finish
8. place your first part and use your drawn rectangle to constrain
the part

9. use the Pattern Parts(!) function on the toolbar and
- select the placed part (when not already selected)
click the green checkmark in RibbonBar
- for the pattern select the created sketch (easier in EdgeBar)
- select the pattern within the sketch
Finish

That's it. Be Warned: when Editing the sketch with the pattern don't
use Edit --> Undo ALL as it will wipe out your patterned parts
(not the sketch) and you have to start over.

dy