A Knowledgebase for all Die Designers…

Logopress has added an extremely helpful warning regarding Splines, Ellipses & Parabolas (AKA nasties). This new warning is displayed when validating the property manager of the Annex part if it finds any nasties in the Blank section sketch. (When creating the Annex part, Logopress3 automatically creates the Blank section sketch and this is the sketch that is used to automatically or semi-automatically create the internal punches and the external punches. It is practically always very important for multiple reasons that this sketch does not contain nasties.)

Here’s how it works:

When unbent it looks like this

When you select Part preparation before strip starting to create your Annex part, and after you select your options in the Part preparation property manager and validate, you will see this warning dialog pop up:

It will highlight the nasties that are in the Blank section sketch and prompt you as shown and you should definitely answer Yes. At this point Logopress3 will create a new sketch at the bottom of the tree that shows the nasties like this:

This is extremely helpful because it shows you all of the areas in your Reference part flat blank that need to be cleaned up. It is important to note that you should not clean them up here in the Annex part, but rather in the Reference part. Open your Reference part and roll back to just above the flat blank station mark as shown here:

Select the Delete face command in SolidWorks (Insert, Face, Delete…) and highlight the area shown below (always be sure to select the option Delete and Patch when working with a solid body) and validate to remove this nasty area in the part. Doing so causes it to be absorbed by the true radius to the right of this nasty area.

At this point you should roll to the end of the tree and do a CTRL+Q (SolidWorks forced rebuild) which causes the Logopress3 body files to be recreated. Now open the Annex part, then select the Logopress3 command from the pull down menu called “Update the stations of the Annex part used in the strip”. This will import the newly created body files and cause the Blank section sketch to get recreated based on the new, clean flat blank. Note that as you can see in the picture below the sketch at the bottom of the tree that Logopress3 automatically created called “Sketch showing the splines on the flat blank” now has dangling relations in it. You no longer need this sketch so you can simply delete it.

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(3/31/2013 – The post below was written in 2010 and since that time Logopress has put in place something to automatically warn the user about splines, ellipses and parabolas if he or she forgets to do what is recommended in the post below. See related post dated 3/31/2013 named “Logopress3 warning regarding “nasty” sketch elements“)

Typically (almost always actually) we want to avoid using splines in our die designs. Just as most CAM software systems do not like working with these complex entities (and some won’t, period) sometimes CAD doesn’t like it either so we really must avoid using them in our Logopress3 strip layouts. Make sure there aren’t any splines in the flat blank of your Reference part and that way you won’t have any in your strip layout or in your wire EDM geometry such as punches, die blocks, etc.

It is a good practice to always check your flat blank at the end of the Reference Part if you think there is any chance that there may be splines in it. If you have already finished your Reference part, along with the last station mark for the flat part, roll back just before it this last station mark. Then, click a face of your flat part and start a new sketch on it. (If this flat face of your model is made up of multiple faces because, for example, an unbending caused a the main face to be split at one of the unbendings, then you should select each of these flat faces until the entire flat blank is highlighted.) Then use the SolidWorks Convert Entities command to convert all the entities around the perimeter of the flat blank. Now we want to see if these are all good entities or not, so we’ll use the Logopress3 command found with the other Logopress3 Sketch Tools called “Convert splines into segments and arcs”. A dialog box will come up in the Property Manager with a suggested conversion tolerance, simply accept what is already in this box by checking Okay. If there are no splines in the converted entities within this sketch, then the sketch will still be black since every segment will still have its On Edge relation that it automatically got from the Convert Entities command. If there were splines, you now have some blue, underdefined entities because these splines have now been converted by Logopress3are into either line segments or arcs.

Now you can either work with this existing sketch to fully define the new lines and arcs and make it nice, tangent geometry, or you can simply save this sketch and close it, understanding now what geometry on the flat blank needs to be “repaired” to eliminate the spline areas on it. For example, if you simply have an inside radius and an outside radius that showed up as being blue (spines that were converted to lines and arcs) it could be as simple as doing a delete face on the solid body blank in the corresponding inside and outside corners and then adding fillets that correspond to what is supposed to be there. Of course these new fillets will be comprised of arcs rather than splines.

You may feel it would be easier to work with the new sketch that was converted and use this new sketch to create your flat blank by fully defining all of this geometry and of course eliminating the splines. If this is the case, then simply fully define all of the entities in this new sketch or create new geometry as needed in this new sketch, deleting the geometry you don’t want to use (or making it construction geometry) and then you can extrude this sketch, being careful not to “merge” it with the first “bad” flat blank. Do a Delete Body on the original flat blank solid body to get rid of it. This method of creating a new sketch and new solid body is particularly a good idea if your flat blank had a lot of bad geometry (splines) in it or if it had one or more split faces due to unbendings and you would prefer to work with a cleaner blank.

(07/26/2010 – I would like to reinforce the fact that this method mentioned in the paragraph above is definitely the cleanest and most foolproof way of handling the flat blank solid that you have in your file just before the last station mark is created. Part of the reason for this is because even though the entities converted into a sketch may all show that they are not splines, it is possible that some dirty geometry still exists on the edge thickness of the solid body. By starting fresh with a new sketch that has no splines that you will be doing a BaseExtrude from, you are guaranteed a good, clean sketch. If this flat blank solid is left dirty, you may end up having problems later including, but not limited to, trying to use the Join command later to create a single solid body for the strip.)

After finalizing the blank, “audit” this blank by doing another sketch on it and converting the entities and using the Logopress3 “Convert splines into segments and arcs” again to check and make sure you have all black geometry. The second audit you should do after this first one is to right click on an edge of the flat blank and Select Tangency since of course we’d typically like to use good, clean geometry made up of fully defined tangent lines and arcs. If it is not important if you have tangent geometry for whatever reason, or if it is okay if some arcs are missing, then of course you can skip this audit.

Once you know that you now have a good flat blank, roll to the end of the tree, past the last Station Mark and then to a Ctrl+Q in order to rebuild this last station mark. If you have already started your annex part and your strip, then switch to either the Annex part or the strip assembly and use the command on the Logopress3 pull down menu called “Update the Annex part used in the strip”. When it asks you if you want to rebuild the Reference part, it is a good idea to answer yes, even though you may have just done a Ctrl+Q while in the Reference part. This assures that the body files will get updated. If you already have punches in the strip assembly, then the sketches will now have dangling entities in them and you can either repair them or delete these punches and remake them.

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Updating the flat blank geometry along with the cutting punches and all of the openings in the die is a very easy process if the correct steps are followed. Rather than try to explain it all here though, I will simply point you to our ten minute long video #9 on our “Logopress3 Strip Layout & Die Design” video series page.

Click here to go to the video

Tips to remember to make your update after development go smoothly:

1. Use the power and automation of Logopress3 to make the change. Don’t do it “manually”.
2. You must make your change to the Reference Part (the part that contains the Station marks) and NOT to the Annex Part.
3. Make your change at the proper place in the tree – it might need to be earlier than just before the final flat blank Station mark.
4. If possible, do a Move face to update the flat blank geometry. This will typically keep you from having to edit the punch sketch.
5. After making the change to the Reference Part before the correct Station mark, roll to the end of the tree and do a Ctrl + Q to update the body files.
6. Open the Annex Part and then click on the Logopress3 pull down menu and select “Update the stations of the Annex part used in the strip”.
7. Answer yes to the rebuild question – this causes the import feature to automatically re-import the newly created/modified body files into the Annex part.
8. Open the strip assembly. Do NOT concern yourself with the tool assembly at this point. Leave it closed to keep yourself from being tempted to modify it.
9. In the strip assembly, if you have modified geometry cut by the punches that involved new sketch entities as I did to the external punch in the video, it will have errors in the sketch.
10. If you did not add or remove sketch entities in the flat blank geometry, but only moved it via the Move face command or changing a dimension on a fillet radius, for example, then everything will update fine on that punch.
11. (It is a good idea to edit the punch that has errors in its sketch, then create a new sketch within this part file by selecting the front plane for example and converting entities (using the SolidWorks “Convert entities” command of course) from the face of the punch to capture the original geometry before you are about to make this change to it. Then, display the relations for that newly created sketch and delete all relations. Then, select all of the underdefined sketch geometry and add a Fix relation so that it is fully defined. Now this newly created sketch is no longer being parametrically driven and it is a good idea to move it to the top of the tree and name it “Original punch geometry before development” or some such thing so that you can remember what it is. This way, particularly if the punch and die have already been wire EDMed, you have this original geometry in the model in case you need to delete all of the sketch entities for the extrude of the punch that is being updated and then reconvert them from this newly created sketch that has no parent. (a dumb sketch, if you will) This is sometimes necessary if the geometry becomes overdefined…)
12. Use the Logopress3 command “Create/Edit a strip layout” and then select the punch that has errors in it and delete the dangling geometry. At this point, it is a good practice for convenience sake to switch the SolidWorks display style from “Shaded With Edges” to “Shaded” – this allows the sketch geometry stand out like a sore thumb from the cut edges of the solid model. It hides those cut edges, making sketch editing much nicer.
13. The “Blank section Sketch 1″ that is in the Strip Skeleton will be visible at this point. After deleting the dangling geometry, select the new geometry that had been changed in the flat blank and use Convert entities to convert them into the current sketch.
14. Validate the sketch and there should now no longer be any errors in this punch.
15. Now, when you switch to the tool assembly, the tool assembly should aut0matically rebuild all punch cuts through all plates.
16. If there were no errors in the strip assembly after following the steps above and in the video, and after switching to the tool assembly there are errors in the punch, you may have to edit this punch cut manually in the tool. The correct way to do this is to convert entities or offset entities from the punch sketch that is in the strip. But typically, correct updating practice will cause the tool to automatically rebuild itself.

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