Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Moving a part

N

Nick C

New member
Ok I'm learning ProE in my spare time by teaching myself , ,,, ok ok you can stop laughing now,,,


I completly baffeled as how to move or rotate a part , I cannot seem to find a way to do it. Reason is that I have some imported dxf that is coming in slighlty angled to the world datums and I would like to move it and centralise it on the origin.I suspect that I do not need to do this as I will position my parts in the assembly , right ? but surely there must be a way to move and rotate single parts in a part design window.


Cheers Nick ,
 
Teaching yourself?
smiley36.gif


Nah, really there are lots of us. Looking at your question; I'm learning something...

There are probably lots of ways, Copy / Paste Special comes to mind (Special allows transforms). What I'd probably do, though, is create a coord sys referencing the default. Drag it above the import feature. RMB the import feature, Edit References. Reroute Feat, Alterate (reference), pick the new CSys. You can now move and rotate the import as you please by re-defining the CSys. (Sumpin' I've wondered about; is it possible to define a reference CSys on import, a config option to be set, etc?)
 
I see, attach a datum plane to the dxf and then redefine the datum plane essentially.


I had tried the copy and paste special and this is exactly what I'm looking for but I don't want to copy it , I just want to move it, ( gimme my Triball !!!!! , infuriating when you could do it in two secs in another program , )
 
" ... attach a ... "

Well, maybe. Be mindful of dependancies and how they are created. If you make a datum feature dependant on the import you won't be able to make the import feature dependant on it; e.g. "drag above". I was thinking more along the lines of making a CSys dependant on a Default Csys (which would be the import's parent).

" ... don't want to copy ..."

Think this'll work if you are using WF2; look at the Independent Geometry feature. Create one (Insert, Independent Geometry). Now do your transformed copy. Edit Def the Ind Geom and (menu) Geometry, Collapse Geometry. Return to part mode and delete the original import feature.
___

Triball? One of my first exposures to CAD was Trispectives. I remember a trade rag article titled something like "The Pro/E Killer?". That sorta stuff was largely responsible for my not ever looking at trade rags any more.
smiley2.gif

Edited by: jeff4136
 
I thought "dxf" filescame in 2D for drawings only, but if they can come into "part" mode, you can do the same thing that I sometimes have to do with "igs" or "step" files.


Create a new part with the default datum planes. Create a coordinate system with these planes. If you need to "skew" the part at all, create another coordinate system,rotating itfrom the first one, at the angle(s) that you need.


After this is done, on the top toolbar, pick "Insert", "Shared data", "From file", and select the "dxf" file that you want to import. When prompted for the coordinate system, select the one that you created. DO NOT let it use the "default" coordinate system.
 
DXF can represent 3D data.

FWIW, instead of creating plane; create a default CSys(0) and reference it to create a second CSys(1). If you have to offset the import feature CSys(0) won't affect model size.

How do you get it to prompt for references on import? I've always had to redefine the refs after import. I'm missing a config opt?
 
When you import data, a small box opens up that lets you select a coordinate system to align the data to. As far as I know, that is the only reference that it lets you select.
 
ok I managed to get it to reroute the feature , and now my imported dxf seems to be attached to the new cordinate system but how do Ichange this coord system to the angle of the import #. I try to redifine the coord system and all the features disappear ! , maybe I define a few datum planes , and pick these up ??? (this is getting long winded)


# i.e. my import is coming in and its about one or two degress off from the world axis, so I want my new coord system to be aligned with this and then I can rotate the whole lot back to the world axis.


(megaladon , kind off , I use Ironcad at work but I'm having a play with ProE in my spare time, so I'm missing my triball very much.... never thought I would say that !)
 
Allen,
I don't get the dialog, WF2. Must be a config opt. I'll dig into it someday.

Nick,
There are probably about a dozen ways to go about it. Use your imagination.
smiley2.gif


Seriously, if you are just starting out with Pro/E your time would probably be better spent working thru fundamentals tutorials. In the process try to fathom how the program works and don't waste time trying to figure out how to get it to do something the way you did it in another program (a sure path to frustration).
 
Nick:


Create the first coordinate system "square to the world", (CS0). Then create a second coordinate system rotated 2
 
I was kinda thinking that this would a be simple thing to do, but obviously its a little more involved. I think that I will continue with the tutorials , and orientate my parts in ironcad !
 
This is not a difficult thing to do. I will try to step you through it as best as I can. Let's start all over.


Create a new (empty) part, name it whatever you want. Pick the "DATUM" icon to create the 3 main datum planes. Pick the "COORDINATE SYSTEM" icon to create CS0. While holding the "control" key down, select DTM1, DTM2, and DTM3.


Nowmake the second coordinate system, CS1. Pick the "COORDINATE SYSTEM" icon again. Select CS0 as the reference. Pick the "ORIENTATION" tab in the dialog box. Pick on the "X" axis" box and enter the 2.000
 
Nick,


Do you use a start model. I.E. part with datum planes, csys, views, units, etc. already established and saved to start_model_dir (Tools/Options). Default path is $pro_stds\templates. If not, here is one:


2006-01-04_151034_start_part_inlbs.prt.zip


Next, for dxf import, (I'm on WF2) ... Insert\Shared Data\From File


View attachment 1560


Next pick dxf from drop down list in Open dialog box.


View attachment 1561


Locate and open dxf file. In the solid options and placement, do not use default. Instead choose the pick box (select) to select the csys from screen.


View attachment 1562


After selecting csys from screen, click OK.


View attachment 1563


I use this technique to create sheetmetal flats from other softwares. Turning 2D dxf geometry into a ProE sheetmetal prtto run in Pro/Manufacture. Depending on how the part was originally created and exported out as dxf might have an impact on placement. This part was originally created 1st quadrent, WorldUCS in AutoCAD and placement into ProEaligns perfectly.


If your part is not aligned (due to poor part creation, software, or dxf export), use Measure Distance to find angle, offset amount. Create another csys using this information and EditReferences of ImportFeature and choose new csys (after you move new csys above Import Feature in Browser).


View attachment 1564
 
The method used above establishes your datums as Parent Features and your import geometry as Children of these Datums which I consider good modeling practices. Remember, ProE is very complicated and flexible. You could use an Empty format when starting a new part (no start part) and create all your Datums (coordinate and 3 planes) off of the Import Feature (inserted dxf or other geometry). But this establishes the Imported Feature as the Parent and the Datums as children. You need to understand Parent/Child relationships and how to fluently create any Datum (csys, plane, axis).


This is similar to what Jeff is implying.


jeff4136 said:
Allen,
I don't get the dialog, WF2. Must be a config opt. I'll dig into it someday.

Nick,
There are probably about a dozen ways to go about it. Use your imagination.
smiley2.gif


Seriously, if you are just starting out with Pro/E your time would probably be better spent working thru fundamentals tutorials. In the process try to fathom how the program works and don't waste time trying to figure out how to get it to do something the way you did it in another program (a sure path to frustration).
Click to expand...


Jeff,


If you use an empty format (no start part or established Datums, csys in this case), you will not get the Placement Dialog box.
Edited by: ncprog
 
If you use an empty format ...
Click to expand...

Thanks, Pard.
I found what the culprit was. I have intf_in_use_template_models = YES. For some reason it keeps the Chose Solid Options and Placement dialog from opening. (I somehow doubt that's a documented feature.)
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top