schetch and measured dimensions are not the same
This difference is well below the tolerance for the sketch solver. I think the sketch solver only guarantees accuracy to 1.0E-6. This is to be expected if you show all decimals in Measure
Jeff Strater
Engineering Director
I am not sure why you are seeing the odd dimension, when I checked your model and sketch, it measures exactly 127 mm out to 8 decimal places.
Maybe keep the sketch a simple rectangle and fillet and shell the extrusion. Still a very small error at the end of the arc but the faces are correct to all places.
Mark Hughes
Owner, Hughes Tooling
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Sorry, been otherwise occupied. First question is: What joint are you trying to create here? The "UHMW 1/4 in small" components are already fully constrained with respect to the body in "Steel tube test". One rigid joint is all that is needed. Are you trying to add additional constraints between these components?
I will look at the design more a little later. But, a discrepancy as small as you show in the images should not cause a joint failure.
Jeff Strater
Engineering Director
Hi Jeff, I have created large assemblies with many components on them. All components are saved individually and linked to the assemblies, similar to the one in the top picture.
When I am constraining some of components at top level, the constrains fails with no apparent reason. While investigating the cause, I realized that there are small differences between the sketch and measured dimensions. For example, in the picture, the distance between the 2 outer edges of UHMW plates should be 5"+1/4"+1/4" however measured value is 139.6999999999999318 mm (5.4999999999999982 "). You can see this only if select "All decimals" as Precision in the Measure window.
If this difference is shown in a very basic square component, what are the chances that in a large assembly with dozens of parts on them I end up with the same (or bigger) difference?
In the bottom picture the cylindrical constrain between 2 components at top level failed. The typical message that Fusion provided does not means anything and I can only assume the problem comes from the that difference.
You mentioned in your post that there is a " tolerance for the sketch solver". Is there a tolerance for constrains? How many decimals you can have different in a constrain before Fusion reports it as failed?
No, that small of a difference should not cause joints to fail. I still am not 100% clear what joint you are trying to create in the design you shared here. But, I did find one that would fail. I tried creating a redundant joint between the countersunk hole and the hole in the main body:
I noticed, by creating axes through both holes, that they were not lined up correctly. They are off by about .15 mm:
So, I looked at the sketches used to place the holes in both components, and they are off by .15 mm as well. Here is the sketch from the plate:
and here is the sketch from the main part:
This is due to the way you have dimensioned those sketches, it has nothing to do with a 1.0E-13 difference in the Measure command.
Jeff Strater
Engineering Director
If you can show me a joint, on the model you shared, that fails, I can look at that joint. You have not done so. Please share a screencast of the joint creation that fails, on the model you supplied, so that I make sure that I'm looking at the same failure.
However, to "focus on the questions that I have asked": No, I have never once, in all of Fusion's history, seen a case where a sketch solver tolerance/measure discrepancy has caused a resulting joint failure. The sketch and assembly both use the same solver. The tolerances are set to 1.0E-06. The discrepancy you showed in the images in the original post was 1.0E-13 or smaller, so should not be a cause of joint failure. Of course, there could always be a case where this is true, I just have never seen one, so to the best of my knowledge, this is not a general problem in Fusion.
All computer math is done to an approximation. Iterative geometry solvers must have some tolerance limit for performance reasons. 1.0E-13 is nearing the limits of double precision accuracy, and can be safely ignored.
Jeff Strater
Engineering Director
yes, misalignment can be one cause of joint failure. If you find misalignment that is greater that about 1.0E-06, then the next step is to try to track down the cause of that misalignment. It can be from any number of sources, I guess. Under-constrained sketches can be a cause, or imprecise distances for other features can also cause this. Sometimes this can be caused by using grid snapping or using the manipulators rather than entering precise values. In my experience, there is not really a general rule to follow, and the process of trying to find the source of the misalignment can be labor-intensive.
Of course, there can be other causes of joint failures. Conflicting joints can be one cause - one joint may remove a degree of freedom that another joint needs, etc.
Jeff Strater
Engineering Director
Jeff, in your previous post you mentioned that less than 1.0E-06" misalignment between features will not fail joints.
That is not true!
There must NOT be any misalignment between joints (Delta X, Delta Y or Delta Z must be 0 as required).
If somebody is running into issues with the joints because the of extremely small difference between features measurements (as seen in the picture) you can fix it in 2 ways:
1. Click and copy the misalignment value (in this case Delta Z), go back to the sketch and add or subtract the copied amount to the feature you need to move. Because the value is very small you will not see any differences in the sketch. However if you done it properly, when you go back to assembly, this time the features will be perfectly lined up and you can make the joint.
2.) Using "Edit in place" project the features that you need from one component to another. Clean the original sketch, create the features again based on the projections and save the component. When you go back to assembly you will see there is no misalignment between the features (Delta X, Delta Y or Delta Z shows 0) and the joint is successful.
In 2016 I have proposed to add "Tolerance" to the Joint window, same as "Measure" window. The reason is that sometimes you want to make a joint that is not very important in term of functionality, instead of spending hours or days to figure out why the joint fails.
If in the last 4 years you got frustrated because how joints work, drop me a note. Together we can maybe convince Fusion to create a better product. Looks like Autodesk start listening to customers only after it receive 2 open letters from important corporations.
