How to change the default insertion point of parts or assemblies being assembled into a large modal

[ptc-4903149]

When initially bringing a part into an assembly using "main Window" mode, but prior to placing the part, can you change the default incoming position relative to the assembly, maybe there is a config setting that allows the new part to appear in the current window, zoomed in to the spot you want to add the new assembly item?

Why am I asking - On large assemblies, the new incoming part enters the assembly model very far from where I want to place it (way off screen).  It takes a lot of mouse work to drag it over to where it needs to be placed. Why am I not using the "Separate Window" mode in assembly? Because the separate window mode is quirky and difficult to use, in my opinion - parts almost always end up upside down or end up being unassembleable forcing one to use the main-window assembly mode.

[ptc-4903149]

After I posted this question, I learned about the configuration option: "comp_assemble_start" which you should set to "move_then_place".  With this option activated, new items will enter your assembly glued to your mouse cursor instead of appearing very far away.  I was also embarrassed to learn that this config option has bee around since the Wildfire days (over 15 years ago), but then I had been using the program before the revolutionary Wildfire version.

HOWEVER - The configuration command "comp_assemble_start" set to "move_then_place" has a drawback.  

Keep in mind that the screen mouse cursor only defines 2 of the 3 spatial locational dimensions meaning that while an incoming assembly item looks like it is near a particular object in an existing assembly, because it is glued to the mouse cursor, it's position relative to the view screen (computer monitor) is not fixed and will, most likely, be very far away from where you think it is along an axis perpendicular to the view screen.

Therefore, before bringing a particular item into your assembly, be sure to use the View "orient" command to rotate the assembly such a flat face on an existing part near the intended insertion point is parallel to the screen.  

Then, when you bring in your item, and after using the left mouse button to get the new item close to its final destination, use the assembly constraint "coincide" to lock one of the item's faces to the assembly face that is parallel to the screen.  This locks the 3'rd coordinate to the desired location.  You will probably then need to delete this constraint and then perform the normal assembly process.

If you don't do this, your item will often disappear from the screen during assembly because the software will not have properly set the 3'rd spatial dimension.

[ByDesign]

Thanks for posting.  Even if you figured it out, the post serves to enlighten.

Sometimes PTC makes things very frustrating.  I found that even as frustrating as it sounds, if I zoom my model to the place I want the new part to assemble, then assemble it by picking surfaces from the parent, and datum planes of the component from the model tree, then I can get the part to the right place, usually in a reasonable orientation (by the way the datums are chosen) without even seeing the component until it is there close to in place.  If I need the part assembled by things other than datums, then I can delete constraints or modify them as needed.  It makes a little more work on the constraining side, but it saves a lot of hassle chasing parts -- especially when it's a small part in a large assembly.

For what it's worth, I did not know about the comp_assemble_start option.  Thanks for sharing.

[ptc-4903149]

Thanks for your kind words.

You mentioned assembling parts using datums. I view this as a dangerous practice since one of the great values of 3D CAD is to evaluate how components fit into a given space meaning that you need to assemble parts as they are assembled in the real world, i.e., you have to check part dimension stack-up (e.g., left side of a bearing's inner race, when pushed leftwards, touches right side of a snap ring and left side of snap ring touches left side of shaft snap ring groove, etc.) Assembling by part or assembly datums can accidently get parts imbedded within each other. It is hard to see a few thousandths of embedment on two given parts, but the error adds up over many parts that touch each other (related issue: part tolerance min/max stack-up).

Back when Creo was ProE, they tried to push the idea of first building model datum "skeletons" onto which you would assemble your parts. The idea was to more easily design, for example, linkages but in reality, this was a bad idea pushed by software people that didn't actually design stuff for a living.

For the record, the assembly I am currently working on is over 50 feet across with thousands of parts, so it was hard to assemble a single tiny bolt onto this. Because I only have worked on such a big model for the last couple of years, and because I am lazy, it took me this long to find this configuration setting that lets parts or assemblies enter the model by being glued to the tip of the mouse cursor.

I realize that for almost forever, Pro/E/Creo has had a separate window showing the new part during assembly where you can click on surfaces on your part and align them with the assembly, but I have found it very easy to flub this up such that the Creo squawks at you saying your constraints are invalid. I have wasted so much time with false starts that I have given up on the separate assembly window mode entirely for large assemblies.

Good luck in your work!

[ByDesign]

I get it.  I'm a long time Pro/E user.  The hiccups involved with datums are many, but as mentioned, it's a simple way to get a part to the right location in the assembly - especially a small part in a large assembly.  For me, a little extra work defining constraints (twice) is easier than chasing parts all over - zooming, etc., for no real reason.

As another idea - it appears they took some of this away in Creo - but, it Pro/E we used to be able to pick all the constraints and features of one part, then zoom to the other and pick the matching features (surfaces, datums, axis, etc.) there. Only after the last constraint was satisfied did the new part pop to its proper location.  I have not tried that with Creo because it has a nasty habit of flipping things or changing constraints if you come back to them. It's super frustrating, but Tech Support says that's how it's supposed to be.  -- Hogwash, they just don't want to fix the problem, but I diverge.  Anyway, you can try it.

These ideas work for some situations, not for others.