How i can round a dimension on the custom unit in drafting? for example I have a dimension "460.12". I want round it on 50 unit precision that show me "450".
I don't know why you would want to do this, but it wo0uld be better to restrict the part itself to the multiples of 50 and not modify the drawing.
You can use equations in the part file to drive this.
In Manage Equations, create Global variables:
MultipleFactor = 50
MultipleCount = INT(PartDimension / MultipleFactor)
MultipleRemainder = PartDimension - (MultipleCount * MultipleFactor)
MultipleRemainderAdder = if(((MultipleRemainder) > (MultipleFactor/2)), 1, 0)
MultipleDim = (MultipleCount + MultipleRemainderAdder) * MultipleFactor
This sets the variable "MultipleDim" to the closet multiple, (optionally) rounding up.
So a PartDimension of "460.12" would make "MultipleDim" = 450
MultipleCount = INT(460.12 / 50) = 9
MultipleRemainder = 460.12 - (9 * 50) = 10.12
MultipleRemainderAdder = if(((10.12) > (50/2)), 1, 0) = 0
MultipleDim = (9 + 0) * 50 = 450
A PartDimension of "475.12" would make "MultipleDim" = 500
In Manage Equations, use "MultipleDim" to equate the part dimension that drives the feature.
SW Drawings don't have equations and it's best that the drawing truly reflect the part.
EDIT: If you wish to just override the dimension's value, select the dimension and in the Proprty Manager, delete "<DIM>" and type in the value you want.
You may get a warning message, but you can continue modifying the dimension value.
Also, on the value tab, you can check to override the value.
EDIT 2: A caution on overriding a dimension (for any reason):
With <DIM> removed form the dimension, the drawing dimension is effectively severed from the model and regardless of all model changes, the dimension will not change.
Additionally, there's no apprearance difference between a dimension that has its <DIM> and one that doesn't.
So, not only must you remember every such dimension and maintain them, you must inform everyone else that these dimensions will not update to their models.
I'm not in front of SolidWorks to test this, but another approach may be to use the fraction option for the dimension.
You can also set the fraction precision for the whole document in Document options>Units.
But as for the individual dimension, this approach may not work for your purpose as the caveats above still apply.
Curently you can ot round the dimension. I'm having the same problem. That is why I created the idea for the Top Ten List Dimension round off in drawing for individual dimension based on specified increments (such as to the nearest 5 or 10)
Please vote, maybe it will be implemented.
Hi Mahmood, here's a dirty little trick that might work for you. You will have to insert the dim into the drawing as a model item, or to the sketch point.
edit: another option I might consider is use a tabulated dimension in a BOM - you have options for precision there.
In the bom list, how to set the decimal digits
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