Shniblets (slivers) in the strip layout

Sometimes you find that after you’ve created a strip layout you are left with a sliver, or shniblet as they say, that that is sitting at die level in each station of the die. Often times, usually that is, the sliver is the result of an angular bypass mismatch on a radius. This would happen if your reference part and subsequent annex part has a full radius and then you add a cutting punch that does not go all the way around the radius but rather shoots off on an angle – an angular bypass mismatch. So you’ve got this teeny tiny sliver left with two straight edges and one radius edge. In the earlier stations of the die when this area of the part is still flat, the sliver is not a problem because it blends in with the part. But as soon as this area of the part gets formed down ninety degrees for example, then this sliver stands out like a sore thumb.

This sliver is in the skeleton part of course, as opposed to being in the annex part. So in the first station that you see this sliver hanging out in space all by itself, click on it. Assuming you have the SolidWorks option checked that is named “Scroll selected items into view” under System Options, Feature Manager, (99% of users do) then the “Strip Skeleton Linear Pattern” expands in the tree and the part in the pattern with the specific configuration that you just clicked on is highlighted within this pattern. Either click or right click on this highlighted part and Edit Part. If you expand this part, you will see that the Solid Bodies folder now has 2 solid bodies in it (assuming all other skeleton parts before this one have 1 solid body). Expand the solid body folder and you probably see the first body being called “Punch Cut…”. Clicking on this body at this point will highlight this small sliver and then hitting delete on your keyboard will put you into the Delete Body command. Validate this command and you will now see a Body-Delete feature at the end of the tree for this particular skeleton configuration and this body will no longer be visible.

Now stop editing the part and get back into edit assembly mode. Let’s say that for this example, this particular skeleton part was named “…Strip Skeleton 1<5> -> (Step 005)” and that after this skeleton part, there are 3 more skeletons in this pattern named 006, 007 and 008. These represent different configurations of the skeleton. So standard SolidWorks functionality causes this Body-Delete feature to show up in each of these following patterned skeletons, but it is SUPPRESSED in each of these following configurations. So you could expand each of these parts/configurations manually and unsuppress this feature in order to make them disappear, but the easier way, particularly if you have many skeleton configurations after this one, is to click on the feature that is at the end of the tree in the skeleton part/configuration that you had just created it in (005) and then go up to the LogoPress pull down menu and select “Unsuppress on the following stations”. This of course will unsuppress this Body-Delete feature in the rest of the pattern, which represents the rest of the strip.