How can I dimension the OAL of a chain consisting of individual elliptical links?

S_Regula

Hi All,
I've created a single chain link that is elliptical in shape with 3.4mm round stock and a 0.5mm gap. I then created an assembly using individual links and a linear pattern to create a full chain. When I drop the chain on a drawing, I am unable to dimension the Overall Length because I can't figure out how to snap a dimension to the outermost quadrant on the end links. Has anyone encountered something like this? How can I accurately dimension the OAL on my drawing? TIA!
 

MichaelPascoe

Try splitting the face of the chain so that Onshape recognizes there is an edge to snap to. Sometimes this helps. Also, try dimensioning anything, then dragging the dimension nodes to the correct location afterwards, this will enable orthogonal snapping, I think there is a shortcut for it too, but I can't remember.

S_Regula

MichaelPascoe said:

Try splitting the face of the chain so that Onshape recognizes there is an edge to snap to. Sometimes this helps. Also, try dimensioning anything, then dragging the dimension nodes to the correct location afterwards, this will enable orthogonal snapping, I think there is a shortcut for it too, but I can't remember.

What do you mean by "splitting the face of the chain"? Do you have an example that I could take a look at? Thanks.

MichaelPascoe

@S_Regula share a link to your document and I'll show you. Within the part studio, there is the Split feature. You can use this to split the face of your chain link into quadrants, forcing it to have an intersection vertex at each end. This should allow you to easily dimension to it within a drawing.

That, or you could create a guide sketch and measure to that, but I don't like bringing sketches into drawings, it's redundant work.

S_Regula

MichaelPascoe said:

@S_Regula share a link to your document and I'll show you. Within the part studio, there is the Split feature. You can use this to split the face of your chain link into quadrants, forcing it to have an intersection vertex at each end. This should allow you to easily dimension to it within a drawing.

That, or you could create a guide sketch and measure to that, but I don't like bringing sketches into drawings, it's redundant work.

I tried the split feature, then created a composite part consisting of the 3 "chunks" of the link. When I drop it on a drawing, the lines shown are very rough and I'm unable to attach a dimension to the actual node location to get the correct dimension (should be 35.6mm):



Any idea how to improve this?

MichaelPascoe

I was referring to splitting the faces of the chain segments, not the part. Either way, you will need to double click the drawing view and change the render settings to "Best quality" and simplification to "None" in order to get rid of the poor draw quality.

S_Regula

MichaelPascoe said:

I was referring to splitting the faces of the chain segments, not the part. Either way, you will need to double click the drawing view and change the render settings to "Best quality" and simplification to "None" in order to get rid of the poor draw quality.

I was able to change the view settings and it improved the view quality. For the chain link, I used a sweep to create the part and then used the right plane in the Split feature to break the part into 3 chunks, then created a composite part consisting of the 3 chunks:



It seems to have worked, although the dimension on the drawing is not exact (keeping the dimension on the drawing to 1 decimal place shows the "correct" value). But, I'm curious what you mean by "splitting the faces of the chain segments, not the part"?

MichaelPascoe

If you edit the split feature, there is the option to split the faces instead of the part. This will keep it all as one part, and only split the faces.

S_Regula

MichaelPascoe said:

If you edit the split feature, there is the option to split the faces instead of the part. This will keep it all as one part, and only split the faces.

Ahhh... I didn't realize that. That eliminates the need for creating a composite part. Thanks for the suggestion!

MichaelPascoe

Yep! I've found that it is also great for creating "Anchors" for the drawing so that the annotations don't break as easily when parts are updated.