I searcehd for and found/read several postings on this same issue. The solutions involved workarounds which I don't agree with.
I derived an assembly. The assy weighed 765.490 kg. The derived part weighs 123.796 kg with material Default, and 971.802 kg with the material Steel.There doesn't seem to be a method to get the originating assy mass to 'automatically' reflect in the derived part mass, other than manually over typing the part mass. This is the workaround I don't agree with.
Anybody got a better idea?
ORIGINATING ASSY
DERIVED PART
The reason for this is fairly clear in your screenshots; Your assembly is lots of parts of different materials, and your substitute model is a single part of one material. Should Inventor carry over things like mass...? I'm not convinced it should. The resulting mass is just the volume of the overall shape x density.
To report the correct mass, I would add a line of iLogic in the source assembly that reads the mass and saves it as an exported parameter. Whhen you edit your substitute part, you can include that parameter from the source file. You can then write that mass parameter into iProperties.mass of the substitute part - thereby creating the "live" link you are looking for.
Hi brendan.henderson,
I might be remembering this incorrectly, but here's something to try. Rather than deriving from a part file. Go to the assembly file and expand the Representations folder, and then right click on the Level of Detail node and choose New Substitute > Derive Assembly. Then step through the dialog boxes choosing the options that apply.
Ok, so after typing the above, I just did a quick search and found this link that gives some information about substitutes and mass props, that supports my recollection:
http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-00B17673-8CC3-4F6F-9CC3-8069F3487C03
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
yes guys from what I can see the mass doesn't stick and maintain throughout derives. I tried substitute parts, and even changing bom type to see if there was some inbuilt sticky function but found nothing. there are probably cases for having it stick or not stick but I would think that we have a case for some better functionality and perhaps on the "physical properties" window, or the "derive part" window, we have a new button called "keep mass from imported parts / assemblies" or something similar to save us having to watch out for this curve ball...
ok so heres the idea posted over on ideas station. kudos it if you aggree.
http://forums.autodesk.com/t5/Inventor-IdeaStation/stick-mass-on-derive-or-import/idi-p/4883574
I understand what is happening also. I just don't agree with it. The derived part begins with a material of Default which equates to 123.796 kg. I changed it to material Steel.
iLogic sounds do-able. I'll investigate that and Curtis' idea also.
I would have thought that a derived part would, by default, get the mass from the source and be blank material or composite or something that has no affecting kg/m3.
Thanks Peter.
I gave your idea a shot. All worked smoothly. I used the Standard.ipt template for this. Switching to the LOD SubstututeLevelOfDetail1 and looking at the mass gives me an NA. Hitting update gives me the prompt about "Do you want to calculate the Mass Props for the Master LOD?" question. I hit Yes and the mass updates and is the same as the assy Master LOD. All good so far. Switching back to Master LOD and looking at the mass and it's okay. Switching again to SubstituteLOD1 and the mass is again NA. And the process repeats. If I were to put this SubstituteLOD onto an IDW the mass value would be NA. Not good.
FYI, step 7 (if the mass properties are up to date and the active LOD is not the Master LOD, you are prompted to copy the Mass Properties of the Master or the active LOD before proceeding.) did not popup so the mass must be okay at the Master LOD level.
Opening the Substitute file created by the above process and looking at the mass, I see that the part has the default material set in the Standard.ipt template file and the mass is 117.980 kg. So again the mass is not correct. Also not good.
I want to use a substitute part because I don't want 2 of my macros processing the parts of the source assy file. They are legacy from 4 years ago and need to be updated which is a long process I simply don't have the resources to deal with now. I simply want a substitute part to represent the assy. But I want it to have the correct mass value without me having to manually type in values.
Thanks for your input Curtis, but unless I skipped something in the help file link it doesn't appear to work.
It appears that it DOES pull the material from the template used and calculates the mass on that. I don't agree with this. It should have a link or something to the originating assy file. Why is the substitute (derived part) required? To simplify it's placement into another assy file. But the mass (and probably COG and other stuff) must be correct or there could be drastic ramifications.
Thanks for you input Blair.
@Blair wrote:
Post it to the IdeaStation...
Hi blair,
Mark_Wigan created an idea for this, see his post above for the link.
On second thought here's the link:
http://forums.autodesk.com/t5/Inventor-IdeaStation/stick-mass-on-derive-or-import/idi-p/4883574
It might be a good idea to add some comments to his idea, to flesh out the details of the idea.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
I know this is an old post but I cant see anything more recent so thought I would chip in as I have been fighting this for a few hours...
If you create the substitute / derived part / shrinkwrap etc as a solid, there does not appear to be a way to bring thru the mass properties of the assembly. If you create it as a surface composite the assembly mass comes thru to the part correctly
If the IAM contained parts of the same material, then when its Derived to a single part it wouldn't be a problem. As soon as you Derive to a single part it inherits the Mass of a single item.
When you create a Surface Composite, you retain the individual items as referenced by the "Composite". The mass for each item is still retained even though they are Surfaces
I had the same problem and this surface method seems to work perfectly. I wanted a simplified part derived off of an assembly to use as a component in another assembly. It was important that it derived off of a central location and retained mass and CG. It opens up alot of possibilities, it's a shame that Autodesk doesn't make a feature like this more prominent or allow it to work with solid bodies as well.
Hi Jordan,
I am glad that you find this workflow useful. The original design intent was for Shrinkwrap/Substitute workflow. It could have been made more explicit and easily discoverable. There is an issue with supporting Solid Bodies in this case. For Composite Body, there isn't a concept of mass prop to begin with. As a result, it is fairly clear that the source assembly mass prop can be carried over. For Solids, it gets a bit more complicated. First, Solids do have physical properties. To support Derived Solids, the mass prop dialog would need to have one additional mode along with computed and manually overridden. This 3rd mode will be for Derive feature only. It would be messy to add additional control which users may not understand. when and how to use it.
Many thanks!
Hi,
My remarks to this topic for Autodesk is:
Derived part and assembly (Copy i-Properties)
Please give your vote and maybe it will implemented in future releases.
Regards |
Regards,
Arthur Knoors
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Please fix this issue that occour only when you derive an assembly with the option 'Surface'!! This cause confusion to the user because the same workflow is perfect if you derive a part. In this last case the mass is zero and it's correct!! The normal use of the command derive with the option 'Surface is to retrieve the geometry to model a new part using another part or assembly as a reference.
Hi! I believe you meant "Single Composite Feature" in the Derive Assembly, right? I recall there was a change in behavior since 2022 (Model States). What release of Inventor are you on?
Many thanks!