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Re: Circular sketch pattern doesn't fully define sketch
That's why a lot of people, myself included, don't use sketch patterns. Why do you not want to pattern the feature?
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Re: Circular sketch pattern doesn't fully define sketch
In this case I'm not making any features, just laying out a pattern for connector clearances.
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Re: Circular sketch pattern doesn't fully define sketch
Greg
Check the "Display instance count" then fix the center of rotation after you make the pattern.
I'm not saying it should work that way, but there it is.
Dwight
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Re: Circular sketch pattern doesn't fully define sketch
I have the display instanc count, how do I fix the center of rotation beyond it being the axis of the circular face the rotation is made about?
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Re: Circular sketch pattern doesn't fully define sketch
Gregory Page wrote:
I have the display instanc count, how do I fix the center of rotation beyond it being the axis of the circular face the rotation is made about?
You have to add it as a sketch constraint after you do the pattern. Doesn't have to be a "fix" constraint; can be anything.
It's the same for a linear pattern. If you constrain one instance of the pattern (seed instance doesn't count) then the whole pattern is fully constrained.
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Re: Circular sketch pattern doesn't fully define sketch
The centerpoint is constrained, still doesn't constrain the pattern. Best I can do is turn-off require fully defined sketch, exit sketcher, then turn require fully defined sketch back on.
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Re: Circular sketch pattern doesn't fully define sketch
when I want to constrain a circular sketck pattern, I make a construction circle. and constrain it where I want the pattern (location and diameter). then I constrain 3 instances from the pattern to the circle (usually the "seed" and 2 others) - essentially defining a 3 point circle. I do it this way because I do not usually like the dimensioning scheme generated by the "add dims" option in the pattern tool.
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Re: Circular sketch pattern doesn't fully define sketch
Greg
If you are on SW2011 or earlier, you can post the part and I'll take a look. If you are on SW2012, post an image?
Dwight
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Re: Circular sketch pattern doesn't fully define sketch
This is the sketch with the pattern. center is the centerpoint of the part face which is also the sketch plane.
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Re: Circular sketch pattern doesn't fully define sketch
Are your seed curves all fully constrained?
Your screen shot shows it during pattern construction. Can you show one just after construction?
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Re: Circular sketch pattern doesn't fully define sketch
Seed curves are fully constrained and that is after completing the pattern creation and verifying the center rotation point is constrained. That's all it will do unless I turn off use fully constrained sketch so it will let me exit sketcher.
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Re: Circular sketch pattern doesn't fully define sketch
Greg
I tried to duplicate your sketch. It may be that the pattern's radial construction lines are sitting on top of your construction lines. If you drag one of the pattern instances, as shown below, it should move the center of the pattern. You may then constrain the two centers and that should fix the pattern.
(I'm not sure how your sketch is not overconstrained. I assume the outer green circle in the image you posted is referenced from the edge of a previous feature. I couldn't add all the dimensions you have without over constaining.)
Dwight
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Re: Circular sketch pattern doesn't fully define sketch
The outer circle is the reference to the existing part, the next one in is a clearance offset. When I select the point at the center of rotation it says it is constrained, and I can't drag the seed or the pattern so i have to assume SW thinks it is constrained too.
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Re: Circular sketch pattern doesn't fully define sketch
Greg
You say you can't drag an instance of the pattern, even though it's blue? That doesn't sound right.
Typically, if a piece of sketch is blue and I don't know why, I'll drag it to find out what the missing constraint is.
Dwight
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Re: Circular sketch pattern doesn't fully define sketch
Yep. It is colored as unconstrained, but you can't drag any of the patterned circles. If I try to grab and drag the point at the center of the pattern that too won't move either and the dialog says the point is constrained.
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Re: Circular sketch pattern doesn't fully define sketch
Okay. Unless I can see your model, that's as far as I can go. Your profile doesn't say what version you are on, but even if it's SW2012, I'm sure someone here would take a look if you posted it.
Dwight
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Re: Circular sketch pattern doesn't fully define sketch
I do what Jeremy suggested and take it one step further if I want the entire pattern constrained you can just dimension
it. I think if I remember correctly this was a suggestion to have patterned sketches copy constraints.
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Re: Circular sketch pattern doesn't fully define sketch
Greg,
Frustrating isn't it. For some reason, some programmer at SolidWorks thought that it made sense to leave the sketch not fully defined, even though the user has input all the information to fully define it. Perhaps, somewhere in the world, there is a user who likes it this way. I have never met one.
Jerry Steiger
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Re: Circular sketch pattern doesn't fully define sketch
If that was the only stupid thing the programmers did I could live with it.
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Re: Circular sketch pattern doesn't fully define sketch
I don't think the people behind the code are trying to be ornery. The pattern only knows relative to itself - it can add angles between its vectors if you check the box (not there in SW10, talking about SW12 - maybe SW11).
But I'm not certain that the pattern generator can determine a "vertical" or "horizontal" sketch relationship - it just doesn't have that context. You and I know that "X" is horizontal. That might be a leap of faith for the code. I'm guessing here. I'm just an oldtime user.
The pattern tool does add a construction line to the dimensioned pattern. All one needs do is add a horizontal or vertical relationship to that line to let the pattern know which way is up.
I agree that it might be darned handy (in the Property Manager dialog for the pattern) to have the ability to inform the pattern which way is vertical (or whatever it would take to fully define the pattern). That would make this extra step seem less extra. Perhaps all the CadJockey need do is check box to confirm "X" is "Horizontal".
In my opinion, they've done some charming things in SW12 - UOM selection is great, Hole Wizard lost its irritating 1st point orphan, sketch patterns are easier to fully define, dual screen ops are almost there, DisplayManager is getting cool, and PV360 is my best friend. These are all the result of feedback from users. I'm hoping this thread will result in another, small but important, improvement in the UI.
Of course, the best way to make suggestions is via Enhancement Request procedure.
Hope I didn't hijack your thread, Greg.
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