’’Simple’’ 3D Model

[andrei2]

Hi everyone

I have a basic 3D model here:
http://img.photobucket.com/albums/v309/Andreii/333d.jpg

I would like to ask:

1. As you can see, Im trying to make this hole but I don't know why proe wants me to determinate both references (primary and secondary). How do I do that? Its not just clicking on one surface of the model. After hard work, I was able to determinate primary reference but whatever I click, nothing can be set as secondary reference. So what is my next step after this (please, look at my drawing - screenshot)?

2. I made a red star on the rectangle. How do I remove this rectangle after 3D model is already made? The surface of this rectangle is Extrude 3 but if I try to delete this rectangle in '' tree view '' then it ''wants'' to delete some more parts of model and not just rectangle. I tried in sketch mode also but I can't even mark (show on rectangle) it there.


Thank you for your answer.

 

[lp.allard.1]

For your hole, you have multiple ways to create it (radial, concentric, 2 refs, ...) but if I understand you well, you just want to create a hole like in your picture, i.e. that is planar... It is normal that Pro/E ask for 2 secondary refs. The primary is used to select the surface where the hole will be located, and the two other ones are used to determine the location on the selected surface (1st ref).

In your case, you should select the middle plane as one of the sec. refs, and the other one, you just have to find it!

For your extrusion, (Ext3) Pro/E will delete only the features based your extrusion. Change your parent-child topology by re-routing some features (Edit Definition and/or Edit references)

Good luck!

 

[skraba]

To select secondary references, click in the area Secondary References to paint it in yellow. Then you can select additional two references Pro/E needs.

Or, you can also RMB one of the handles on the hole start and then select Secondary References Collector. Now, you can select secondary references.

If you don't select Secondary References Collector (i.e. Secondary References window), Pro/E will be changing primary references till you don't select Secondary References Collector.

But, it would be logical for Pro/E to automatically switch to secondary references collector after you pick primary reference, since you would probably know where would you like to put the hole.

 

[andrei2]

Thank you for your answer but I didn't understand what do you mean?

Hole: With determinating where I would like to have a hole, I actually determinate primary reference but it isn't so ''easy'' for secondary reference. If I do the following steps:
- move the cursor on the surface where I would like to have secondary reference
- open ''right'' menu with clicking right mouse button and keep it pressed for about two seconds
- choose (in this menu) Secondary reference
then it deletes even primary reference and I have to choose it again - I get the message Select 2 Items - as is showed on the screenshot.

If i try to determinate secondary reference with clicking (once) left mouse button on the surface where I would like to have secondary reference, it moves the hole on this surface, so it crashes the position of the hole - where I would like to have it.

For your extrusion, (Ext3) Pro/E will delete only the features based
your extrusion. Change your parent-child topology by re-routing some
features (Edit Definition and/or Edit references)

I can't delete this rectangle only from Editiong definition / editing references. I use Wildfire 3.0. There I am able to change only dimensions. I can see the Delete option in the right mouse menu but this option doesn't remove rectangle only.

To select secondary references, click in the area Secondary References to paint it in yellow

Hmm Im not able to click on submenu (in this case, menu is Placement) Secondary References because its actually the name of menu but I think you meant that I need to click on entries what Secondary references contain. I can't click there because it ''doesn't want'' to stay clicked / pressed, it automatically unclick itself.


I tried to search on google.com alone for some more information about how to make a hole but nothing useful... I just saw that determinating both references isn't enough, you need to determinate (after you determinate referenceS) 1 item too (message ''Select 1 Item'' in menu Placement in submenu Secondary References'').

 

[vlad1979]

Hole command works like this: you select primary reference and then click on a surface. Then select second reference and select 2 references (make sure to hold CTRL when selecting those 2 references)


2006-12-15_111048_hole.rar

 

[andrei2]

yes but setting references doesn't work for removing the rectangle. I think the dashboard in Hole Tool is for holes only. Thank you vlad1979 for showing me this video but I think I can't remove the rectangle (which is marked on the screenshot with red star) in the model from this board which i get with clicking on '' Hole Tool '' icon.

 

[vlad1979]

It looks like you made that rectangle by mistake and then all the other features that are after the rectangle have references to that rectangle. So in order to remove only that rectangle you should see what features are related to that rectangle. The best way to do this is to right click on the rectangle feature in model tree and choose parent/child something (I dont have PRO-E at home so I'm talking what I can remember, I'll get back on this Monday morning). So if you find that parent/child a window will popup and will let you know to which features that rectangle is related to. Now let's say a hole or something has as reference a side of that rectangle. In order to delete the rectangle whitout deleting the hole too you should redefine that hole to have other plane as reference. instead of that side of the rectangle.


See if you can redefine the features that are after that rectangle, to not have any references to it.


If you can't find the parent/child you can simply right click on the rectangle feature and choose delete from the list, the other features will be marked for deletion as well, see which one is first after the rectangle and that is one feature that has references to the rectangle, Try to redefine it.

 

[andrei2]

I have seen that ''Delete'' option in right click (on rectangle) menu already but if i click on delete, then it doesn't delete just rectangle but some other parts (the big hole which is in the shape of U) too.
So, if I understand you correctly i need to determinate again the location of those two holes which are in a shape of circle? But I would like to have the location of those two holes exsactly this as I have now (as it is showed on link).
I found Parent / Child option without bigger problems, so I could open ''Reference Information Window'' but I don't see anything here what could be useful in my problem.

 

[vlad1979]

OK now I have PRO_E. Let's redefine something. You have something similar like the movie below.


I have a cut done in the center of my part and then I made a hole which I related it toa side of that cut. Well, you have an extrude but the principle is the same. If you see the movie when I want to delete the cut the hole is selected for deletion as well. So I need to redefine the hole to give it a new reference instead of that side. So I selected a plane which I now it's not related to that cut. After this I can delete the cut.


Now, you have something similar, click on that extrude in the model tree and then right click it and in the menu select delete. See which is the first feature selected for deletion beaside the extrude. If you see my movie, you will see in my model tree the extrude and the hole are selected for deletion. So I know I should redefine the hole.


After you see what feature is first, redefine it so that it doesn't have any references to that extrude.


Repeat these steps until you have only that extrude select for deletion.





2006-12-18_011040_redefine_hole.rar

 

[andrei2]

Vlad your case of deleteion was much easier than my is. You showed me on the video what you were trying to delete and you could delete that with right mouse button / ''Delete'' too. What if I ask you: You had three edges in your part which you would like to delete, is it possible that you delete only left and upper one, so this ''free space'' will be in a shape of ''L'' but changed for 180 degrees? I have been trying to delete the rectangle only, for several times but when I clicked on Edit Definition, it crashed holes.. When I tried to use the function Edit Definition, it threw me into sketch mode.

 

[vlad1979]

Try to redefine the holes first and use some default planes for references. I think you made your holes giving them as references edges from that rectangle. So right click on your hole then click redefine, delete all the references, primary and secondary, and now redo thereferences like I said usesome default planes. Or try to use some faces that are not related to that rectangle.


And you can't delete edges, those are edges from features, you can only delete features, not single edges.


Merry Christmas and see you after the holidays.


PS: If after the holidaysyou still have problems with deleting that rectangle, post your part and I will delete it and make a video to show you how.

 

[andrei2]

Hmm somehow I finally removed this rectangle but not on the way as you told me. In the sketch mode, I put one more rectangle, bigger one and then on extrude tool, I clicked on icon ''Extrude on both sides of sketch plane by half and specified depth value in each direction''. So now, I had half of the length (bigger rectangle) on the left side of smaller rectangle and other half of the length (bigger rectangle) on the right side of smaller rectangle. Then I removed the material and it removed the whole size of bigger rectangle and into this bigger rectangle was the smaller one which i wanted to remove.
By your opinion, could be this way ''acceptable'' too?

Merry christmas to you too and also happy new year.

p.s.: I like your proe's background. Its very nice for my opinion.

 

[vlad1979]

From what you say you made a cut to remove a feature that you couldn't delete it. This is not very "PRO-E".

You should still try to remove that rectangle by deleting the feature that made the rectangle. If you like I could remove it for you, well I could try. Post your part and I'll try to delete it.


About the backgroung there is nothing special, it's the good old pro-e background. You can set it from view/display_settings/system colors and in this window select this:


View attachment 2965


The default grey colour of wildfire isn't for my taste

 

[andrei2]

this cut makes some damage on the surface (it removes very little part of it) and its very hard to create so little part on the surface back.
Thanks for offering me that you could delete it for me but rather not because I make those 3D models for learning proe and since im beginner, I won't sell models or give them to anyone, I will delete them after they are make correctly... With creating models, I learn proe. So if you do something for me (but thank you anyway) won't have any effect on my learning - with this, I don't mean your videos (record desktoping) of course.
I have been trying to delete the feature for few days now but still no success... Can't delete little rectangle only.


Edited by: andrei2

 

[AHA-D]

Looks to me like you are struggling with the basic concepts of "history based, parametric design" like ProE is one.


History based means that you design by adding features, one after another and that new features are linked to previously created features and geometry. From what I read you are trying to work in "direct editing", which is the way that Solid Designer or Autocad 3D works. This definitely is not the ProE-way.


If you first make a cutout and then make a hole into the surface that was created by the cutout, then the two are linked. The hole looses its reference (the plane where it starts) when you delete the cutout. Next, if you refer to the side surfaces of the cut to position the hole, then the hole also looses that reference when the cutout is removed. So what can you do ? Redefine the hole so that first it is made starting from the original surface and not the surface from the cutout. Next, define the position in relation to the base datum planes (they are first in the tree so they always "stay alive"). When this is done there is no reference left to the cutout and you can safely delete it.


Robust design - in any history based modeller but particularly in ProE - is always to be very carefull with you references and only choose features as a base when this helps design intent. For instance if you want a hole through all you can better start it from a base datum plane than from an existing plane of the model.


Alex

 

[vlad1979]

I understand. You can't delete it now, but you'll find one day how