Unable to calculate/update physical properties (imported part from McMaster-Carr website)

[Gabriel_Watson]

See attached. Original part was imported from this (tried as 3D Solidworks and 3D STEP, both did not work after importing into Inventor 2020.4.2):
https://www.mcmaster.com/1078N33/

Rebuild All and changing materials did not work. When we go into iProperties > Physical > Update, there is no change either.
I also repaired the (overly simple) geometry and also tried unstitching and stitching it back on. Then tried finally to add another feature and delete it, which also failed to make any difference.... ended up having to use a workaround of rebuilding this part from scratch in a new file.

I just wanted to understand if there was something I missed here, or maybe leave this up as a good sample for the Inventor devs to look at. Thank you!

[RNDinov8r]

Wow, that is a jacked-up file. Even in 2022 I couldn't get it to update. Looking at the file, it's "construction" seems odd...it shows a single solid body, but it will highlight in sections about 3" long, each.

I can say, unless the mass and inertial properties are absolutely essential, this is one case where we would extrude a rod, and add threads to the outstide of the rod. 

I wonder if those helical forms are messing things up?

[RNDinov8r]

So, playing around with the file, I did get it to display a mass and volume.

I "drilled a hole".

Then I filled the hole, once I did that, it performed a mass calculation. I suspect the mass is for the core, not the entire part, which if that is correct, means IV is not recognizing the original volume.

I played around with the core diameter, thinking that it was measuring the mass of the core, so I went from Ø3mm to Ø6mm and the mass remained the same at .361 pounds (I used one of our materials in our library). So, for whatever reason, that does something. INterestingly, I used a freeform mod on one end initially, and it had no effect the mass calc.

[Gabriel_Watson]

Thanks, maybe your ID change got lost in the bermuda triangle of mass and never recalculated the change... I tried adding a hole then filled it up now with about 5mm ID on the entire length of the item and the mass is still at zero. I find it amusing because it is a simple part, but since we receive lots of parts from McMaster-Carr here, and often customers will send STP/SW files, I figured I should try and get to the bottom of this.

[RNDinov8r]

we use a TON of stuff from MMC....it's actually good to know about this issue. We design a lot of custom End of Arm Tools for SCARA and 6-Axis robots, and mass and inertia are critical for correctly running those robots at high speeds...and we use a lot of MMC stuff on those in some cases...so this is a good find.

[johnsonshiue · Accepted solution]

Hi Gabriel and Chad,

This is a bug. The geometry checks good. But, the coil face with many turns may be too complicated to compute the volume. There is a simple workaround though. Use Split command and select YZ plane or XZ plane -> check All Faces. After that, the mass can be evaluated.

Many thanks!

[RNDinov8r]

Johnson, thanks for the work around. 

Do you anticipate this being something that will get fixed in the next update for 2022?

It's a good discovery either way, because we use so many files from MMC, I'll make my team aware.

[Gabriel_Watson]

Thanks Johnson, nice trick for me to keep in mind too... the only problem is that this workaround requires you to keep that split feature in, you cannot delete it after.

[SBix26]

When I need to use threaded components from McMaster Carr, I typically use the Delete Face w/Heal to get rid of the modeled threads.  It is a very quick procedure to perform, though if you want to truly get rid of the extra baggage in the file, you will want to also copy the solid body to the construction environment and back (also not a lengthy procedure).

The same technique also works with other "over-modeled" features from MMC such as knurling.

---

Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[Gabriel_Watson]

I tried this now, but with so many faces and the pattern on those, I have to keep deleting a ton of surfaces to then try to "heal" it with a boundary patch between the two caps. Is that what you usually try?

Please let me know if you have a minute free to try on this part (preferably, download a new one instead of the sample import I posted originally).

[SBix26]

I downloaded a new copy of the file from McMaster Carr, and tried my Delete Face technique (be sure the Heal box is checked).  Because of the patterned nature of the thread surfaces, I ended up window selecting the whole part (all faces), then deselecting (ctrl-click) the major diameter face and the two end faces along with their chamfers.  This resulted in a cylinder with chamfers.

This threaded rod is just as easily produced by modeling it from scratch, but the technique applies to all kinds of threaded items from MMC. 

I checked file sizes after each operation:

  STEP file: 12,626 KB

               V

ipt after conversion: 3,285 KB

               V

delete face w/heal: 2,019 KB

               V

Copy Object to construction and back, add threads and material: 105 KB

For what it's worth, I was surprised to find in McMaster Carr's web site that one of the choices for download format is "3D STEP no threads"-- sounds as if they may have had some complaints about the heavy files.  Have you noticed that?

---

Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[RNDinov8r]

Yeah, we have been using that option for a while. As a rule though, threaded rod (not screws or the such) we would normally make as a cylinder, apply chamfers to the ends, and then apply external threads, internally ...we wouldn't down load the file.

[Gabriel_Watson]

Right, the option is there for no thread download, I would guess for lightening the load on processing the geometry, but it works for avoiding these issues as well. I am just trying to understand what can be done here in a simple format since we deal with all sorts of bad geometry from customer product data as well.

I am not sure which faces you kept for OD, because the ones I tried did not work. The chamfers are a bit irregular to use somehow:

If I leave just the caps (green checkmark below) and delete/heal 46 faces I get an error, and if I include the next ones (deleting/healing 44 faces) then my resulting geometry does not make sense anymore:

[SBix26 · Accepted solution]

For the Delete Face feature, select everything except:

See attached file (2020 format)

---

Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[johnsonshiue]

Hi Folks,

I do see this issue from time to time. It happens more with complex geometry. Over the years, some cases similar to this have been resolved but quite a few have not been. I am sorry I cannot guarantee a fix.

Many thanks!