Hello, I´m new on Creo, actually working with version 5.
I came from Solidworks and I want to know the equivalent command to "exclude from bill of materials" / "envelope" on Creo.
The idea is to use parts (or sub assemblies) that are not taken into account for the BOM, but serves as a reference to position some other components in the assembly.
Thanks in advance.
In our assembly designs, we use two methods.
1. Add a filter to the repeat region that drives the BOM table. See the attached picture. We have a parameter on each part called Order_Code. We use this parameter to group parts of the same material type within the BOM table. We chose ZZ to be the value for excluding from the BOM.
2. Create a simplified representation that shows only the items you want to include in the BOM. Use that simplified representation to drive the repeat region in your BOM table.
The method in Creo for repeat region BOMs on the drawing is to use TABLE, REPEAT REGION, FILTER, BY ITEM, EXCLUDE and then pick the bom table lines you want to exclude from the BOM.
If this is something that is always excluded, you can set up rules for filtering, as the other user stated.
thanks for reply but the solution of "hide" the component on the drawings It does not work in my case, since it must be represented as "envelope" also on the 3D model (because 3d models are used by other persons and they must know that maybe some parts are not included on the BOM and also on the physical assembly).
The solution by now is to put the "envelope" component as normal part/assembly, then put the other components, make it FIX and the delete the "envelope" component. Its so time consuming and gives issues when you changue something on the "envelope" component, because the real components of the assembly are fix in the space (and therefore the position is not updated).
I don't think you have stated your problem in a way that we understand what your intention is.
Are you trying to manage the BOM and exclude items from the BOM or are you trying to control your assembly when you sometimes want to use an envelope part and sometimes want to use the real model?
I believe possibly you need skeletons which is how Creo will drive position of components and their references without actually using references from the assembly/parts.
I may be way off in my interpretation of what you need so please accept my apologies if I misunderstood.
Sorry, maybe the title was a mistake. "exclude from BOM" its the way that SW call it on the assembly. It have two options, one is "exclude from BOM" (the component is shown on the assembly like normal component but not on the BOM), and the other one is "envelope", who is "exclude from BOM" + make the component semi transparent and green (to clearly see that there is a "reference" component.
What I want to do is not "hide" the component on the BOM, just want to have that component (part or assembly) on the assembly at least (SW gives the option also to show it on the drawings with special type of line, but I no need that in this case) to use it as reference to position / design other components.
I have heard about skeletons but I do not understand clearly how it works. Maybe Im wrong, but from what I have seen, skeletons require both some reference sketch or a "convert" process to use a existing part/assembly. Is there any way just to insert a part/assembly into the assembly Im working and said to Creo: this is a reference component just to place others, please show it in a different way (color or transparent) and not take it into account for the BOM?
Im new on PTC but Im still surprised of how the "easy, simple and direct" features on SW turn it into complex /time consuming processes on Creo.
I miss the "REAL" 3D sketches, multi component mirror/pattern, mirror component orientation, "transparent view of components", folders /sub folders on the tree, assembly component relations in any order (that is one of the worst things in Creo), imported parts auto-repair feature that works, auto scale sketch when you put the first dimension, copy-paste of sketches, etc.
Yeah, what you're looking for is a Skeleton part. It's automatically filtered from the BOM and is used to make reference geometry. If you put solid materials in it it's also excluded from the mass properties, and surface geometry in it is automatically blue (as opposed to the normal purple). You can create it inside the Assembly by the "create" function, choosing "Skeleton part" as the type (I don't have Creo on this computer, so let me know if that instruction is insufficient).
If you want to use several skeleton parts, you need to turn on an option called something like "allow_multiple_skeletons".
As for comparing to SW, Creo is clearly inferior in user friendliness, though it's been getting better with recent versions. Pretty much all the stuff you mentioned can be done quite easily in Creo without too many clicks (and even fewer if you use functionality like mapkeys and UDFs), but you've got to get used to the functions and workflow of Creo. Everybody prefer the CAD system they "grew up" on, get annoyed at the missing features in the new system and don't notice the new features that are available, since it's not part of how they're used to working.
can someone explain me how to create and use squeletons? but anyway I think is not the same as I want, because on SW you just insert any part/assembly and you choose the option to "use as reference". As I understand, on skeletons you must create that type of special component first.
I think the issue with Creo is that the software have the 90s concept in the 21 century…, lot of thinks are complicates, non logical, non smart, non automatic I think because they still working in the same way as old software.
The CAD companies are lucky because its so difficult for the Companys to changue between different softwares (non file format/features standard by now…)
Im not necessary want to do it in the same way of SW, but yes to get the same result. That s why I asked how others work with assemblies but any one seems to be working like this.
I will try the process you said, but seems to be too complex (time consuming).
I will check copy geometry and Shrinkwrap (I dont know anything about that).
According your experience, if you are working with a complex / multi options machine project, how you position the parts refferenced to main machine assembly?
As I know, the most used solution on PTC is place it on the main assembly, then make it fix. It works but if you change anything on the main assembly then the "fix" sub assemblies remain outdated… (more manual work to re update it)
Another issue on Creo is the (bad) support...
3D Sketches: Not as quick, but using datum points and a curve through points, or drawing two 2D sketches and intersecting them is pretty easy. Add some mapkeys or a UDF and it's even quicker.
Multi component mirror/pattern: Group the components and you can mirror or pattern to your heart's content, though I prefer using reference patterns, which are much nicer to work with, and very quick to create.
Mirror component orientation: https://www.youtube.com/watch?v=4rw2zvU0JMk
Transparent view of components: Model display -> component display style -> transparent. I put it on the popup menu (along with "shaded" to turn it off) so it's a simple two-click to activate.
Folders/sub-folders on the tree: That would be groups, though it's true that you can't nest them.
Assembly component relations in any order: I don't know what that means.
Imported parts auto-repair that works: Yes, the IDD could need a revamp. There's quite a bit of manual work needed, though there are tricks and options that help the process a lot (like setting the accuracy to match the STEP). Creo is good at handling native data from other CAD systems, though, so I often just ask for the original file instead, which tends to work better than going through a STEP.
Auto-scale sketch: Use the Modify tool with the "lock scale" option for this. That'll scale your entire sketch.
Copy-paste of sketches: Guessing you mean inbetween features or similar? You have to enter the sketch, select all, then make a new sketch and paste it there. If you're using external sketches, though, it's simple to copy and paste them as you like.
Certainly not saying that all of this is as quick and simple as in SW (I have barely used SW, so I don't know the details), but I, having grown up with Creo/ProE, don't find these things cumbersome at all (except maybe the IDD). And you're probably missing some Creo functionality that's missing in SW. But by and large, my understanding is that SW is a lot faster and easier to use for regular, simple modeling of parts and assemblies, whereas Creo is more powerful when it comes to optimization algorithms, parametrization, automation, and such topics. Not being very experienced with SW, though, I'm not sure.
Its funny because we use a 3D cad software but we cant do 3D sketchs…. (80s technology…)
Datum points are not 3d sketch at all, are time consuming, limitated, and you must use a lot imagination to create things with that. 2020 year and we still thinking in a 2D way….
The mirror feature (new one also) its a **bleep**. Sometimes I dont want to make a group just to make a mirror. Why I cand just select 2, 3, or 20 parts and do the mirror? make no sense.
Also, there is nor posible to select the "orientation" of the mirror when you use the "reuse" option, I mean, sometimes you do the mirror operation and the part its flopped on the wrong position. SolidWorks gives the option of 4 "positions" when you do the mirror, so you can orient it in the right way. This must be done manually on PTC and you break the link between position of the main part. If you edit the position of the main part, you must edit the mirror part also. Time lost...
Transparent components doesnt exist on Creo, I mean, if you turn to transparent, all assembly makes transparent. On SW you just select the part (or sub assembly) and just that part turn to transparent.
Groups is nor the same than folders and sub folders on the tree.
Assembly components in any order: On Creo, you must pay lot of attention on the assembly to the order of the components, because the mates are **bleep**. Also if I delete one "top" component, the software isnt enought "smart" to break the mates to the other components and not delete it also….
Auto repair at the end requires a manual work. Time lost.
Copy paste on sketch doenst work, if you want to reuse an existing sketch you must create it into the "palete". On SW its just copy paste.
I dont think Creo its more powerful than SW, as I see its just more "dummy" soft with old way of work methods. Not customer oriented, not productivity oriented. We are in the 4.0 era and we still working like 20-30 years ago...
Not surprising, Creo is still eons behind Solidworks. It seems like every solution listed on this forum involves silly little workarounds that generally involve mapkeys and finding/changing archaic parameters, which leads to extreme wastes of time. Repeat regions? Give me a break. Solidworks handles all of this with a check box. I think the Creo programmers prefer to spend most of their time creating paramaters rather than truly fixing their substandard CAD package.