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Modeling of a parabola

samfisher

New member
I've created a parabolic shape frame using a datum curve. I used the 'use edge' command in extrusion to select the curve as one of the entities and then simply sketch the remaining part. The problem I'm getting is that after extrusion, I see the curve separately from the edge of the frame (please see the picture below). When I create a drawing of this part, I see the curve as a hidden feature. This is also visible when selecting hidden view in the model itself. Why is this so?
 

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That should be a display issue, just bump up the edge quality in your config options, see here. also set shade_quality to 10.
 
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that is funny thing. I have Creo 2.0, and I encountered same issue.

Ok, that is the story:

I set all edge display settings on highest level on default Configuration panel File > Options > Entity Display. I set even 4x Anti-Aliasing and the results.

At the end I got was the same results as you described with your parabola. Point is, driven factor is edge_display_quality in config pro which was set on "Normal" level.

I just don`t get it - how it possible that Creo has options that do not match each other?
 

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I haven't messed with config.pro file a lot but i think Creo/ProE gets its config pro file from multiple locations (folders) and merges all of them into the session, then if you have conflicting options,in different config.pro files, it may cause problems and inconsistencies like that.
 
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I don't see it as a display issue, because I get a difference is dimensions when I use the curve and the edge. I actually have to manufacture the frame, therefore I need to an accurate dimension. And secondly the curve appears as hidden line.
 
maybe your datum curve isn't planar. then you project into your sketch and that gap appears. can't say much whitout seeing the part. tightening the accuracy settings may work too.
 
ok, i drew a parabola using an equation datum curve and recreated your case. when you project the curve into your sketch, it approximates it with a spline, if you tighten your accuracy settings, it uses more points for the sketch spline and thus you have a more accurate representation. see this image,notice when i tighted the accuracy by 50% i have more spline points and no visible gap: (click to get a larger pic)
%5BUNSET%5D.png
 
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Ok, I got the accuracy concept, and I reduced it to the minimum, 0.0001. The difference does reduce but is still there. My curve is in x-y plane. Does this mean that no matter what, there will be always a difference, because if we consider the spline as a curve with varying radius, then there will be a limit as to the smallest radius pro e can generate.
 
Is the deviation anything critical here? there's always approximation involved,in CAD, in CAM, etc. don't be too picky about it unless its really an issue.
 
The deviation is not too critical, and yes I do not need to be picky. Thank you for your help. There is one other thing I need to ask, I can't find any edge quality config options in the tools>>option. In fact I can't find any configuration besides a few.
 
Here they are:
view>display settings>model display>edge/line>edge quality
view>display settings>model display>shade>quality
or:
in tools>options you should enter the options manually and give them a value. use the find button there, search for quality, the first results is "edge display_quality", set it to "very high" then "add" it. Third search result is "shade_quality", set it to 10 and "add".
 
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This is(check attachment) what I`ve got n Creo 2.0 with edge_display_quality set to very high
 

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