I have been having some difficulties ever since switching to 2018 (so far i do not view it as an upgrade)
todays issue is regarding a "failure due to geometric conditions"
I have attached the model and the slot with which i am trying to split the part - or cut extrude - or surface extrude the slot and cut with that.
all fails
can anyone suggest why this is not working ?
Need to split the part both directions with the drawn slot
Thanks
Brant
You want to cut slot?
like this?
I could only cut it using 2 cut extrudes,
was getting same error msg "failure due to geometric conditions" when trying to cut in 1 go through all both directions.
Probably ZTG issue
thanks - didnt try that
I can do that as a workaround but i actually needed to split the part
what is ZTG?
Zero Thickness Geometry
"SolidWorks does not allow zero thickness geometrybecause it can lead to mathematical problems and downstream errors in the model. Every edge of a solid body must have exactly two adjacent faces. Zero thickness occurs when you attempt to extrude a cut tangent to a hole"
ZTG=EVIL
Hi Brant,
I'm sharing this not only to help with your specific problem, but so others can see a good troubleshooting technique for geometry issues like this.
I believe this is due to the split trying to make very small pieces of sliver geometry, perhaps zero thickness but I cannot say for sure by visually examining it. To test this out, I tried various values for your 6.2mm diameter on the slot. It works if the diameter is <=6.1575mm or >=6.3545mm. If you try any value in between those values, it fails. I have included a modified version of your part that I used to test it out. What I did was to change the diameter value to something that worked to add the split and then I used a move/copy command to move the larger body out of the way so I could easily look at the results of both the larger body and the smaller body(ies) independently. Then I kept on changing the values, first at 0.1 increments, then 0.5, then 0.1, then 0.05, etc. until I figured out the upper and lower bound of where it worked. Then you can look at each body and see what geometry is likely causing the problem and I've labeled that "Very thin geometry" with a note in the model. I also added 3 configurations in the model with the different values. So, if you open the file, leave it in the view I saved it in, and go to the ConfigurationManager and switch between the 3 configurations, you'll see what I've shown in the images below:
Diameter=6.1575 mm
This is the largest size that works below your desired 6.2 mm
Diameter=6.3545 mm:
Notice the very thin geometry. So trying to split at 6.2mm (or anywhere between 6.1575 and 6.3545) is trying to split through this very thin face. There are actually a total of 4 of these thin faces including the other 3 locations around the model where it is being split). Also notice that at these sizes, the result is 2 bodies being split off from the main body.
Diameter=6.5339 mm
This is the smallest value where the result of the split is two bodies instead of three (one body being split off from the main body). You can see the two halves are just barely connected at the top and bottom, by two very thin slivers of geometry. Increasing the value above 6.5339 will give more material connecting the two halves.
So, the modeler is having trouble cutting that very thin geometry. Again, it could be zero geometry, but without developers diving into it deeper, I cannot say for sure since it is hard to tell from visual inspection.
But, is this really the geometry you desire? Do you desire it splitting into 3 bodies or do you really want 2? How are you going to manufacture this extremely thin geometry and is the thin geometry really intentional? If neither of these is the intention of your design, then you will either have to change the dimensions or position of the slot shape which you are using to split the main body or change the geometry of the main body where the slot shape intersects it.
If this really is your intended geometry and you really do need it split at exactly 6.2mm then you will have to submit the model to your VAR so they can work with our technical support team to look into it further.
Thanks,
Jim
Thanks Ned and Chad for the responses.
Thanks Jim for your in depth reply
I get the zero thickness issue.
I had looked for it but obviously not in the right place
It would be great if the software could mention zero thickness when that is the issue rather than "geometric conditions"
I can change the dimension to something that doesn't fail - there is no need to pursue this issue further
Brant
Hi Brant,
It would be nice if you would mark Jim's highly detailed description of the problem you had on your part as being the "Correct Answer".
This will make other forum viewers that have the same or similar problem more likely to look at this post - since it would show that the problem was answered correctly and would be more likely to give them the solution or at least a better direction to solving the same type problem if they have it. I, and many others, have battled the ZTG issue and sometimes, as in this case, it hides and may cause a failure that is very hard to identify. Jim Wilkinson gave a great answer with great and easy to follow details that help see those small marginal features that create problems.
Hi Rick
thanks for the pointer - I do not spend much time on the forum and do not understand the etiquette
Hi Brant,
I'm sharing this not only to help with your specific problem, but so others can see a good troubleshooting technique for geometry issues like this.
I believe this is due to the split trying to make very small pieces of sliver geometry, perhaps zero thickness but I cannot say for sure by visually examining it. To test this out, I tried various values for your 6.2mm diameter on the slot. It works if the diameter is <=6.1575mm or >=6.3545mm. If you try any value in between those values, it fails. I have included a modified version of your part that I used to test it out. What I did was to change the diameter value to something that worked to add the split and then I used a move/copy command to move the larger body out of the way so I could easily look at the results of both the larger body and the smaller body(ies) independently. Then I kept on changing the values, first at 0.1 increments, then 0.5, then 0.1, then 0.05, etc. until I figured out the upper and lower bound of where it worked. Then you can look at each body and see what geometry is likely causing the problem and I've labeled that "Very thin geometry" with a note in the model. I also added 3 configurations in the model with the different values. So, if you open the file, leave it in the view I saved it in, and go to the ConfigurationManager and switch between the 3 configurations, you'll see what I've shown in the images below:
Diameter=6.1575 mm
This is the largest size that works below your desired 6.2 mm
Diameter=6.3545 mm:
Notice the very thin geometry. So trying to split at 6.2mm (or anywhere between 6.1575 and 6.3545) is trying to split through this very thin face. There are actually a total of 4 of these thin faces including the other 3 locations around the model where it is being split). Also notice that at these sizes, the result is 2 bodies being split off from the main body.
Diameter=6.5339 mm
This is the smallest value where the result of the split is two bodies instead of three (one body being split off from the main body). You can see the two halves are just barely connected at the top and bottom, by two very thin slivers of geometry. Increasing the value above 6.5339 will give more material connecting the two halves.
So, the modeler is having trouble cutting that very thin geometry. Again, it could be zero geometry, but without developers diving into it deeper, I cannot say for sure since it is hard to tell from visual inspection.
But, is this really the geometry you desire? Do you desire it splitting into 3 bodies or do you really want 2? How are you going to manufacture this extremely thin geometry and is the thin geometry really intentional? If neither of these is the intention of your design, then you will either have to change the dimensions or position of the slot shape which you are using to split the main body or change the geometry of the main body where the slot shape intersects it.
If this really is your intended geometry and you really do need it split at exactly 6.2mm then you will have to submit the model to your VAR so they can work with our technical support team to look into it further.
Thanks,
Jim