New in SolidWorks. Building family table of SHCS and I want to add mate references for easier assembly of bolts. No matter what I do, when SHCS is inserted into assembly, only concentric mate (1st mate) works, second mate (coincident) does not work. If I place coincident as first mate and concentric as a second one, then coincident mate works but concentric mate (as second one) does not work. Am I missing something?
Try changing the alignment on both mates to "any".
Still the same. I have selected threaded part of the bolt (cylindrical surface - no real tread) as concentric and bottom surface of the head as coincident. When I insert bolt and point to any cylindrical surface it snaps and after I left click it asks me to confirm selection on pop-up window and no option for second mate.
You need to do one mate and then select another set and mate those..
Since you're using Socket Head Cap Screws, see the attached on one of my files - I created all my files per diameter and attached is the 5/16-18 Screw...
John, is your model 2016 version? it says "Future version file".
2017 - however you can go to 3dcontentcentral.com and type in my name in the search bar and look for earlier versions there...
Dave,
I hoover over cylindrical surface and concentric icon shows up next to the mouse pointer. Then it asks me to confirm selection which I do. But then, it does not give me option to select other constraint.
Danilo,
Just checked the way I set up ours years ago as I remember having this issue and what I did was to select the edge between the face and the shaft, set up as below.
Drag and drop it in the assembly over a washer that's already there and I get the mates as such
Btw, i don't have to confirm the mates either they just auto snap in place.
Regards
Stevie
Steven, thank you for reply. I did as you are proposing and it did work. But, I do not like how it behaves in assembly. I always miss the right hole with this solution.
Hi Danilo
Mate References only work for the 1st reference- it is Primary, OR Secondary OR Tertiary rather than all 3 being satisfied. If you use the edge between the flat and cylindrical face, this will capture both the concentric and coincident mate just like how toolbox parts are setup.
if you want all 3 references to be captured and used, then you also need to create a mate reference on the receiving part WITH THE SAME NAME and then SW can match all references- see this video from about 45 seconds
SOLIDShots- Using Mate References - Free SOLIDWORKS Tutorial - YouTube
Adam, that is the answer I did not want to hear ...
So, how SolidWorks, with this concept, works if you want to place a bolt in a hole that is obscured by other detail? I cannot use "Select Other" while inserting component with this method.
Danilo, it is always trying to detect a item to mate with so if you have something in the way, it needs hiding, or your intended part to receive the bolt needs isolating. If the holes in the assembly are made with hole wizard then perhaps Smart Fasteners are the way to go.
Adam Hartles wrote:
Hi Danilo
Mate References only work for the 1st reference- it is Primary, OR Secondary OR Tertiary rather than all 3 being satisfied.
That statement is not correct. You absolutely can get all three references to work.
Please remove the correct mark from that answer. We don't want false information being marked as correct on these forums.
Scott, so even with the second part of the statement justifying what I said? Or is there a way of getting all 3 to work without having to do a pair of matching mate reference names? How about if i Edit to ...
"In your example, without a pair of matching mate references on the receiving part....
the mate reference will only work for the 1st reference- it is Primary, OR Secondary OR Tertiary rather than all 3 being satisfied."
Scott,
I will unmark solution as "correct" but so far, Adam's statement supports what I have experienced with SolidWorks. Unfortunately though.
Also, Steven Richmond, refers to it as a problem he had.
Do you know how I can constrain a bolt using at least two predefined mates (concentric and coincident)?
Thank you everyone for your help!
Here's a zip file with a bolt and washer, and an assembly with the two mated via the mate references. I did just two references in this example, but I could have added a third and it would still work.
There are a few nit-picky things to getting this to work right. The mate references have to be exactly the same in the two files. They have to have the same name, the same primary, secondary and tertiary references, the references have to be in the same order and of the same type, etc. Any difference in the mate reference in one file as compared to the other, and it won't work correctly.
Scott, thank you for taking time to further explain this.
I fully understand how you did everything. And I understand how all three mates work together when I want to constrain two details against one another. The problem is that if I want to add a SHCS into assembly, to do it your way I will have to match each hole with every SHCS and that would be almost impossible to do for whole assembly. Steven Richmond's solution will work for my SHCS the best but it has one small problem: you have to be able to see the hole in order for the SHCS to know how to mate with part. There is no option for "select other" available to go through assembly and pick the right hole that is hidden behind other parts. I do not understand SolidWorks logic behind this, letting only first mate work and second and third not (as per Adam Hartles' comment).
Hi Danilo
Mate References only work for the 1st reference- it is Primary, OR Secondary OR Tertiary rather than all 3 being satisfied. If you use the edge between the flat and cylindrical face, this will capture both the concentric and coincident mate just like how toolbox parts are setup.
if you want all 3 references to be captured and used, then you also need to create a mate reference on the receiving part WITH THE SAME NAME and then SW can match all references- see this video from about 45 seconds
SOLIDShots- Using Mate References - Free SOLIDWORKS Tutorial - YouTube