Using Parameter on Circular Pattern Quantity?

[oregondunerz]

First time posting on here and I am mostly a newbie with Fusion 360, so I apologize in advance if this is a silly question.  

Here is my issue/scenario:  I created 5 parameters in my design;

1. MyOD = 12" -- I will manually change the diameter here

2. MyThickness = MyOD-.75" -- The idea is if I change the OD of my circle the distance between my outer/inner circles will remain the same

3. MyCircum = MyOD * PI -- Gathering the circumference of my circle here

4. MyCircle = .25" -- The 'grooves' in my design will always be .25" diameter - I realize that creating a parameter for something that will always be that size is unnecessary, but just doing it for consistency right now

5. MyGrooves = round(MyCircum / .75") -- I need to spacing to be close to .75" between gooves regardless of the diameter that I select in step 1 above, so they are rounded to the nearest whole number

My process is that I create 2 circles.  The first circle dimension is set to 'MyOD' and the second is set to 'MyThickness', this give me the expected result.  Then, I create another circle that is coincident to the 'MyOD' line and I set it to 'MyCircle', this also gives me the expected result.  This is where it gets messed up though, after creating 'My Circle' I use the trim command and split the circle in half (I suspect this is where I am messing up), and I also trim the 'MyOD' line as well, this is the profile that I want to actually circular pattern around the OD.  I click on circular pattern, select my half circle that I want to pattern, type 'MyGrooves' into the quantity box, which in my example should pattern a total quantity of 50 (round(MyCircum / .75), but it will not allow it.

I realize this is likely a very simple design process for others but I been stumped on this for days now haha. There is 10 better ways of accomplishing this I am sure. Hopefully this makes sense though!  The idea behind all of this is that I only have to draw it 1 time and in theory it should automatically update the total number of grooves based on the OD that I input.

[laughingcreek]

generally, you don't want to do a sketch pattern.  pattern the face.

check your parameters and make sure mygrooves is unitless.

[oregondunerz]

Thank you for the reply!  I tried selecting 'no units' in the parameter box and now my expression stops working for some reason.  If I leave it on 'inch' units the expression works just fine.  I will try to pattern the face and see how that works!  Thanks again,

[laughingcreek · Accepted solution]

I assume MyCircum is in inches.  you have to strip that out in your expression so the result is unitless.

round(mycircum/.75")  

note the division by inches in the above expression.

[oregondunerz]

WOW.  Of course!  I was able to get this to work perfectly and it automatically updates the number of 'MyGrooves' based on the selected OD of the circle, just like I was trying to accomplish.  Much appreciated!  A 14" OD circle will have 59 grooves and an 8" OD circle will have 34.  Perfect.

Another silly question really quickly if you do not mind.  Now that I created the sketch, extruded the body, and circular patterned the face like you suggested, how can I export this completed file to a .dxf?  I am familiar with .dxf export when you right click a sketch but now that some of the features on also on a body that export will not work correctly, right?  I am sure I can figure that one out if you don't have the time!  Thanks again so much!

[laughingcreek]

Just create a new sketch, project the face of your solid into it, and create the dxf from the new sketch

[oregondunerz]

Thank again @laughingcreek !