Hello there, I use ProE Wildfire.
I have assembled 2 components and I have made one component active so that I can modify it. I want to fasten the 2 components together. For that I want to create a set of holes in the inactive part over the active part. When I try to choose a reference to create holes I have no clue how to proceed further to draw datum curve for cut protrusion. Hope the question is clear for you to help me. Thanks, Shankar.
Shankar, in your assembly, go to the model tree, select the model that you wish to change, RMB 'Activate' from the menu. You can now create any feature in this component in the normal way, with the 'Insert' menu. The somewhat obscure part may be in the setup ~ to make sure that datum references, such as axes are available in the part you wish to reference. If you merely wish to reference hole edges in another part, pick near the feature, click the right mouse button to cycle through features and surfaces you may reference.
Hi, I have created parts in assembly mode using other pars as reference. In this situation I have a plate. Behind that I have another plate which has got a few cylindrical protrusions with blind holes in it. Some how the reference is not highlighted and I don't have a view to select the protrusion. The active part envelops the protrusion with blind holes.
I have a drawing. I have created BOM (using repeatregion) and Balloon (thro' repeatregion). The part names are random (I named it randomly). I want to change the part names in the BOM without the Balloon getting deleted. I changed the name by removing the repeatregion and all the Balloons got deleted. I created them manually. Is there a soln to this problem?
Thanks, Shankar
: Some how the reference is not highlighted and I don't have a view to : select the protrusion. The active part envelops the protrusion with : blind holes.
I think a light bulb just went on ~ sounds like maybe you're having difficulty with the new Wildfire selection process. Maybe you miss the old RMB cycle through a query select list. Well, it's still all there, just repackaged. Preselect in the area of the geometry you want to reference, RMB click cycle through the geometry below; or prehighlight, then RMB the menu and select 'Pick from list' which will give you the old QS list of features Pro/e can drill through under the mouse pointer. If you can't pick the geometry you want, as always you help yourself out by zooming in (Ctrl-drag MMB)
: I have a drawing. I have created BOM (using repeatregion) and Balloon : (thro' repeatregion). The part names are random (I named it randomly). : I want to change the part names in the BOM without the Balloon getting : deleted. I changed the name by removing the repeatregion and all the : Balloons got deleted. I created them manually. Is there a soln to this : problem?
First, this depends on how you created the part names that are referenced in the BOM. If you had created them as parameters, you could have edited them in the BOM table just by click-highlighting them, then editing the values. If instead, you've used the asm.membr.name, these are taken from the system as the names of the files from which the assemblywas constructed. You could, with the drawing, assembly and parts in session, rename and save the parts and have the names of the components update in the drawing BOM. Or you could do this a level lower, in the assembly, with the parts in session, saving the parts/assembly. Then open the drawing, and the BOM should pick up the new values for asm.membr.name. Or, you would simply replace the format to which the BOM was attached and the new BOM would update with the new values. Once the new values in the BOM successfully regenerate, place the baloons again with 'Table>BOM Baloons' and pick the repeat region. Select whether to place 'By view', etc. and DONE. And, none of these involve doing it by hand.
David Janes
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