When a want a circular repetition 4 times 45 degree on 360 degree, SW give 5 holes , one on the center of my circle. Why?
Marie-Ève Morin wrote: I draw a circle of reference , snap my first drill (9/16) on .After in the edit mode in drill operation, I choose circular repetition.I choose 4 holes on 45degree on 360 with same space between each.After ok, I have 5 holes on my function. Not 4 Its a bug, I think because when I chose circular repetion after I make only one drill on my cicle ref. Its ok.
Marie-Ève Morin wrote:
I draw a circle of reference , snap my first drill (9/16) on .
After in the edit mode in drill operation, I choose circular repetition.
I choose 4 holes on 45degree on 360 with same space between each.
After ok, I have 5 holes on my function. Not 4
Its a bug, I think because when I chose circular repetion after I make only one drill on my cicle ref. Its ok.
I wouldn't agree that this is a bug.
I would say that this is a function of the sketch circular pattern command.
It generates its own center point for the pattern (and you're not permitted to select the origin even if it's coincident to the pattern center).
And any point in a hole wizard sketch will become a hole wizard entity.
There is no distinction between a point used for "reference" and a point indicating the center of a hole wizard entity.
This idea to have a dedicated hole wizard point (a separate entity from the normal point) was one of the Top Ten 10 ideas posted last year, but it didn't get enough votes to make the top ten.
If you wish, you can submit an Enhancement Request (ER) to SolidWorks to implement this idea.
Go to this post: SolidWorks Enhancement Requests and watch the attached video on how to add an ER and to first search to see if it has already been requested.
Please do not reply to this post. It will do nothing to add your ER. It's just a handy link on how to create an ER.
Lastly, I agree with what Mr. Schroeder mentioned about performing patterns after the hole wizard for situations such as your post.
Modifying the pattern is much easier than doing so within the sketch.
Attach the file.
Soft data, hard conflicts.
Marie-Ève Morin wrote: When a want a circular repetition 4 times 45 degree on 360 degree, SW give 5 holes , one on the center of my circle. Why?
We'd like to help but we need more information. How were the hole locations specified?
It looks like you drew a center rectangle for your hole wizard sketch to locate your points on the corners.
The center rectangle contains a point at the center intersection of the construction lines.
This point is what's being displayed in the center of your part.
You can delete the center point from the center rectangle but this also deletes the relations that maintain the center rectangle behavior.
As others have shown, locate hole points using other sketch geometry.
You can also locate just one hole point, then exit the hole wizard command with just this one hole and then use a circular pattern for the other holes.
4X will still be the hole callout count using this method.
EDIT: If my notion about the center rectangle is correct, then I believe the callout quantity will be 5X even though one of the holes is in empty space.
Hi Marie ,
First of all , position the first hole at the proper location .
Next , while going for circular pattern mention the no. of pattern , axis & feature to pattern correctly .
As per now these two conditions are enough solve the problem ...if not please ping up again...
Something like this?
When reading your post I had the same thought that Kevin Chandler expressed; that you'd used the Hole Wizard. I thought I'd share my Hole Wizard workflow with you in case you're interested. When I use the Hole Wizard it's frequently to place four holes in a rectangular pattern, so I almost always create a separate stand-alone sketch first. Then when I'm in the Hole Wizard function I place the points coincident with the appropriate points in my sketch. I've done this for years and it works well. It adds one more thing to the feature tree, but for me the advantages far outweigh that small consideration.
I don't currently do it this way, but I see the advantages. I think I will try it going forward, thanks! Feature trees can always be cleaned up by folders if they get too wild.
Were you creating a circular sketch pattern? Although some people will disagree, I recommend avoiding sketch patterns completely. It's easier to control, and easier to edit later, if you create one instance with your sketch, and then pattern the body or feature as a separate function.
+1 on Glenn Schroeder's and Kevin Chandler's advice.
Always pattern features, not sketch points. Much more stable.
Why you don't follow the correct steps
SolidWorks circular pattern - YouTube
Tutorial SolidWorks 04 - Circular Pattern / Mass Properties - YouTube
Some people made the correct steps you must follow that if you make another thing you have another results but, did you want another results?
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