How can I have sketch lines drawn to perfect lengths. I mean it should be in multiples of 1/16 of an inch.
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Solved by jletcher. Go to Solution.
Are you talking about in a model sketch or drawing sketch.
Are you talking about something other that creating a line, dimensioning it to a tight precision and then measuring it and it is different then what you inputed?
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I am talking about model sketch. I need to know if there is something like a autoCAD snap to every 1/16 points. So matter what I draw, it would measure in multiples of 1/16.
If you turn on Snap yes and to control the spacing go to sketch in Document settings and there is a snap space setting.
I would go with what James suggested. I think that is the best avenue to take.
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I'm not trying to say this should not be done, I'm questioning why someone would want to do this?
I'm falling back on the training I had for Solidworks 2000 yrs ago and still practice to this day with Inventor.
I was taught way back then to not attempt to draw something exactly the way you what it, to draw something over or under exaggerated then come back and apply constraints then dimensions to "perfect" the sketch. At least when it came to model sketches.
As Scott did, I'd go with what James recommended to accomplish this as easy as possible, especially if you desire exact increments, but will add that you should be able to type in the length of a line while drawing it, ref where 0.606 is shown below. Granted, this doesn't provide the snap to grid option!
I've never once used snap for anything (besides AutoCAD). I draw my sketch to plus or minus around 20% scale and constrain from there, regardless of what parametric sofware I was working in. I'll trust a dimension that read 2.1875" long before I trust that I snapped to just the right spot.
I think its more a personal choice. I would want to draw a rough sletch and auto dimention.
@CAD-One wrote:I think its more a personal choice. I would want to draw a rough sletch and auto dimention.
I would strongly urge you to rethink this approach. Auto-dimensioning does not capture your design intent, symmetry or important constraints. It just gets everything nailed down as it is, but with no logic in relations of one element to another. If you have to or want to modify the sketch, you have a big mess to deal with.
For keying in fractional dimensions, you can use, for example, 4 13/16", and it will be retained in the model exactly like that. Sometimes useful where it's nice for a later user to know that you designed it to a nominal value, not necessarily to four-place precision.
But, for quick and dirty, the grid and auto-dimensioning will get the job kinda done.
Sam B
Inventor 2012 Certified Professional
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still waiting for a foreshortened radius dimensioning tool in Drawing Manager
I too concurr with what is being said. I have turned my grid off. Never use it.
I like to sketch things then dimension them and adjust the dimension to what I need it to be.
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@mrattray wrote:I'll trust a dimension that read 2.1875" long before I trust that I snapped to just the right spot.
To add to what Mike wrote, While you can set your system to snap to grid, all that is is a graphical thing in that it helps you locate where your cursor is going to snap to. It does not guarentee in terms of applying a constraint or dimension, that your line is in fact located at or begins where it snapped to.
What I'm getting at here is just because your mouse cursor snapped to a location on the grid, Inventor is not doing anything to ensure your line does in fact start or connect to that specific spot. Only with constraints and/or in combination with dimensions does that "lock down" where exactly that line begins at.
Understand or did I muddle it up more than needed? LOL
That's why you're seeing alot of replies here stating they don't construct sketches in Inventor that way, unlike the way we all used AutoCAD yrs ago.
James,
Yeah, I know. I turn them both off. I know they are different, but I consider them the same because in
my line of work I don't have a need for either. Not that you would know that.
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