Swept Blend Problem.

[lliw2]

Hi, I am modelling a steel pole tower.





It is 25m tall, top diameter of about 182mm, bottom diameter of about 511mm.



I used a swept blend, I am trying to make it have a wall thickness of 5mm, but
I get a warning (see image)



http://img152.imageshack.us/my.php?image=piczj7.jpg



Does anybody know how too get around this?



Thanks.



Edited by: lliw2

 

[kdem]

Try entering a value in the range you are given and complete the feature. Then select the feature and right mouse click>Edit and change the thickness to 5 then regenrate to see if ProE will accept the value.

 

[lliw2]

I just tried that, it didn't work. Thanks anyway.

Someone told me to change something with tolerance's but I didn't really understand what they were talking about.

Anyone else got ne ideas?

 

[design-engine]

do it in two steps. Get the blend to go and shell it or create another blend inside.

dont give up tho.

 

[lliw2]

Thanks, got it.

the shell didn't work but i did another blend inside.

 

[tobbo]

the problem is accuracy!! Change it and it will work

(look under : edit - setup - accuracy)


Pro/e makes a box around the complete modell , and then it calculates the "longest distans" inside the box (in other words, the distanse between one corner to another...) . Then pro/e takes this distans and divides it whit your accuracy value ( default 0.0012) and thevalue you get it the "smallest" value/distanse/lenght you can have in your modell.


So, if you change your accuracy , you can have a smaller value , in your case "5" .


but , you will get a heavier cad modell....


Good luck!!


//Tobias
Edited by: tobbo

 

[jeff4136]

> Someone told me to change something with tolerance's but
> I didn't really understand what they were talking about.


Slog thru ...
[url]http://groups.google.com/group/comp.cad.pro-engineer/browse_ thread/thread/7ac7b385bb720124/24fc891e008c7ebe?lnk=st&q =#24fc891e008c7ebe[/url]
... and the linked docs and you'll know all about it.
(Search for "dynamic" if you want to cut to the chase.)


If you're on maint there are several informative KB articles related to
accuracy / system tolerance settings and issues.


And then, fwiw;
"I am given to understand absolute accuracy will be the default
setting in WF5, so this sort of problem should go away."
[url]http://groups.google.com/group/comp.cad.pro-engineer/browse_ thread/thread/76104510fabf8530/dd2923e5948e4438 [/url]

 

[jraquet]

The accuracy is probably the problem. With this you should be able to make a thin part or shell a solid.


You can alsomake a surface feature and then thicken.

 

[lliw2]

Thanks, This forum is a great place!

 

[rudresh.hm]

hi will,


as rightly said by tobbo, this is a problem of relative accuracy. Any edge less than (length of the cuboiddiagonal * relative accuracy) is considered short edge, so feature generation fails.


you can creat it as a solid or a surface, I think thickness isnot an issue here at all. i think this is just for representation. even you are not going to creat drawings of it, because nobody can manufacture a 25m long single piece pole!!!


you may consider it doing as an assembly, if the thickness reallymatters toyou. you can have a skeleton part with surfs only. make apublish geometry surfacesand each individual parts created using this copy geom surfs and required thickness given in part level.
Edited by: rudresh.hm