Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

DERIVED PART MASS NOT CORRECT

21 REPLIES 21
Reply
Message 1 of 22
brendan.henderson
2707 Views, 21 Replies

DERIVED PART MASS NOT CORRECT

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

MASS1.jpg

 

 

 

DERIVED PART

MASS2.jpg

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

21 REPLIES 21
Message 2 of 22

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.

Peter
Message 3 of 22

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

Message 4 of 22

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

best regards,
- Mark

(Kudo or Tag if helpful - in case it also helps others)

PDSU 2020 Windows 10, 64bit.

Message 5 of 22
blair
in reply to: Mark_Wigan

A good one to post on the Idea Station. Have the option to retain the original Parents mass and CoG for the derived part from an IAM. I can understand what is currently happening as in now becomes a uniform single material item. It would be like having a crankshaft where you have drilled out holes and pressed in a Tungsten insert to balance the shaft. The volume of the crankshaft hasn't changed but the mass and CoG has. By the Derive to single part you in effect eliminated the balancing process and the CoG has changed as well.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 6 of 22

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.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

Message 7 of 22
blair
in reply to: brendan.henderson

It would/should pull it from the default setting for the template used. We have a number of different default templates for IPT parts, so it could be whichever template we pick to start the Derive Part.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 8 of 22

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.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

Message 9 of 22
brendan.henderson
in reply to: blair

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.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

Message 10 of 22
blair
in reply to: brendan.henderson

Post it to the IdeaStation, at times it would be nice to have an override at the time of doing the Derived. Other times it would be nice not to. If you have a fitting/fixture that can be made in a number of different material but with the exact same shape. Simply selecting the correct Template for the start of the Derive would produce the correct Mass. Both options have merit and there should be an option for both.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 11 of 22
Curtis_Waguespack
in reply to: 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

 

Message 12 of 22
blair
in reply to: Curtis_Waguespack

I've given it a thumbs up and added some additional request/enhancement.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 13 of 22
stephengibson76
in reply to: pcrawley

Hi, I would also like my substitute to have the same mass as the parent assembly, makes sense to me, the substitute is a cut down representation of the assembly, not a part in its own right???

Stephen Gibson



View stephen gibson's profile on LinkedIn


Message 14 of 22

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

Stephen Gibson



View stephen gibson's profile on LinkedIn


Message 15 of 22
blair
in reply to: stephengibson76

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


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 16 of 22
jordan.littlejohn
in reply to: blair

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. 

Message 17 of 22

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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 18 of 22

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

Autodesk Affiliations:

Autodesk Software:Inventor Professional 2024 | Vault Professional 2022 | Autocad Mechanical 2022
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!


! For administrative reasons, please mark a "Solution as solved" when the issue is solved !

Message 19 of 22
gusi_cl
in reply to: brendan.henderson

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.

Message 20 of 22
johnsonshiue
in reply to: gusi_cl

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!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report