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Pattern

you need to select those two sketches, right click and select group, then pattern the group.
here's a video showing this.

* the reason you may not be able to pattern sketch 4 and 5 correctly is that you have not selected good references at one of their endpoints. what i would do is edditing sketch 4 and delete the reference to Curve:F17 and instead make a reference to a datum point with ratio of 0.5 on that curve. then make a coincident relation between end point of the sketched arc and this new reference point.
here's what i mean (the same goes for sketch 5)

Edited by: solidworm
 
I looked at it also. You can't have a radial pattern without a starting angle. You have the sketches attached to a feature. You have sketch 4 drawn on the Right Datum. You need to create a new Datum attached to the axis and referenced from the Right datum at an angle, could be zero (0).
 
Thank you very much Solidworm.Maybe you remember.This is your second help for me.The first one was a similar design.I also have the same problem one that one.Now I understand the main problem.Please tell me what is the general approach to solve these kind of problems.I also thank britineeng and radelectronics for their interest.
 
yes i remember!
smiley1.gif

sketch 8 can be axis patterend for me without problem.
as a general rule,you have to keep, references you make in the seed sketch of the pattern as robust as possible. patterns in ProE are somehow adaptive. i mean it tends to keep and apply the same references and relations you make to neighboring geometries in the seed sketch to other instances of the pattern. if you don't need this behavior, you can use "geometry pattern" feature. it's in edit menu. it only copies the seed sketch and rotates it around the axis without caring for references.
for example for the part you have attached in the first post, if you select sketch 5 and goto edit menu and select "geometry pattern" and change the type of pattern to axis,then select the axis, it will do it without a problem because it will ignore references and only copies the geometry as is, and patterns it.


Edited by: solidworm
 
Dear Solidworm,
I did it at last.But as it can be seen the reason that I make these patterns is to to make boundry blend .This is the shoulder of the jar.But this time I cant make boundry blend.Please help me again.Of course the last step is patching .Best regards.2010-10-08_134434_o_t_67.prt.rar
 
sgokben,
the trick i used on the part you posted a few weeks ago, does not work on this one. i suggest to trim side surfaces like the picture below and fill that 6 sided surface.i'd like to do it but it's tricky and requires a lot of time.so i can't do it. you can search the forum for "n-sided surface" posts and see how they build this kind of patches.
for the boundary blend, it's best to work with single segment curves instead of curves that have multiple connected segments like connected arcs and lines. so you might want to replace them with single segment splines. also if you cant make a single boundary blend to cover the whole 360 degrees around your part, you can use symmetry conditions for your model and build some 4 sided patches using boundary blend,mirror or pattern them to make the required surface.
6sided.jpg




Edited by: solidworm
 
no,i made that six sided patch in solidworks, it can be done in wildfire too, but it takes more time because it should be modeled with a number of boundary blends.
 
first you need to merge all those surfaces together, the result will be a single quilt in proe language. but surfaces need to be tied together on their edges,if there are gaps between them, you can't merge them. in your part, there is a gap between surfaces at the bottom corners. if you have decided to make the corners with non-tangent 1 and 2 surfaces, you should make the base(surface#3 in the image) with tangency break as well.
gap.jpg

it makes your work harder and your bottle look odd. (the neck of the bottle already looks odd)
you can still add a fillet like surface to make it look smooth like this:

it will make the bottle look better and the rest of operation easier. would you like to do this?
fillet3.jpg
 
I checked the model and I found some other gaps.What can I do to get rid of them?If the reason is accuracy of lines nad radiusus do I have to increase it and how?
 
there are gaps at the bottom of the bottle bottle. it's not because of accuracy. it's because the buttom surface is made by a boundary blend that has only direction one curves. if you could include the loop of edges which 2 of them is shown with crosses in pictures above, as direction 2 curve of that boundary surface, that gap would be closed. but it's a good solution at all. do you want hard edges on the corners or do you want them rounded like the last picture above?

if you want to see a smoother representation of your model you can go to:
view>model display>edge/line tab>edge quality and set it to high
view>model display>shade tab>quality and set it to 10.
 
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