Updating or changing the part after development or other part change

This is, without question, the most important post in our knowledge base.

Changing a strip layout and even a complete die design is a very easy process with LogoPress if the correct steps are followed. In order for it to be an easy, automated and painless process it is important that you make these changes as outlined below.

Note that this information below applies whether you are simply updating the flat blank geometry (along with the cutting punches and all of the openings in the die) after development or if you are making a customer engineering change to the part.

Besides explaining it carefully below, we also demonstrate making changes to the part in the ninth (9th) video on our “LogoPress Strip Layout & Die Design” video series page. This video is less than ten (10) minutes long. We strongly encourage you to both watch this video as well as read the steps below.

Click here to go to the video

1. Please do use the power and automation of LogoPress to make changes to the part. For the smoothest and most error free outcome, if you have LogoPress, then do NOT make changes to the part “manually” in SolidWorks.
2. IMPORTANT – before making any changes to your error free tool assembly at this point, we suggest that you zip your assembly before making any changes in case you have problems. That way you can get back to where you were before starting to make changes. This is especially important of course for new or relatively inexperienced users.
3. You must make your change to the Reference Part (the part that contains the Station marks) and NOT to the Annex Part.
4. Before making any changes to the flat blank geometry, it is a good idea to have a reference sketch in the tree so that you retain a record of what you had before making the change. To do this, create a new sketch within this “Reference Part” part file, either before or after the last Station Mark, and convert all entities from the face of the flat part including any internal openings that will be changing. Then, display the relations for that newly created sketch and delete all relations. Then, select all of the under defined (blue) sketch geometry and add a Fix relation so that this new sketch is fully defined by way of fixed entities. Now this newly created sketch is no longer being parametrically driven. It is a good practice to rename this newly created sketch something logical that has the current date in it, for example: “Geometry before change on 1-2-2016“.
5. Make your change at the proper place in the tree – if you are just updating flat blank geometry after development, the change will take place just before the last Station Mark, whereas practically all other changes such as engineering changes would be put in the tree before the first Station Mark.
6. If possible, do a Move face to update the flat blank geometry. This will typically keep you from having to edit the punch sketch because you are just moving existing geometry and not creating new geometry.
7. 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.
8. Open the Annex Part and then click on the LogoPress pull down menu and select “Update the stations of the Annex part used in the strip”.
9. 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.
10. Open the strip assembly. Do NOT concern yourself with the tool assembly at this point. It is best to have the tool assembly closed at this point to keep yourself from being tempted to modify it manually. If you did not add or remove sketch entities when you changed the flat blank geometry in the reference part, but only moved it via the Move face command or by changing a dimension on a fillet radius for example, then everything will have updated without errors in your strip.
11. If you have no errors in your strip assembly at this point, you are good to go and you do not have to read further. You should be able to open your tool assembly and not see any errors in the tree.
12. If you have modified geometry in your reference part in a way other than Move face or by simply changing a dimension, then one or more of your cutting punches will have errors.
13. If you have a punch that has errors in its sketch, it is a good idea to have a reference sketch in the tree of that punch part file so that you retain a record of what you had before making the change that you are about to make. To do this, edit the part using SolidWorks (do not edit it while in the LogoPress “Create/edit a strip layout” property manager) and create a new sketch on the front plane and convert entities from the face of the punch. Then, display the relations for this newly created sketch and delete all relations. Then, select all of the under defined (blue) sketch geometry and add a Fix relation so that this new sketch is fully defined by way of fixed entities. Now this newly created sketch is no longer being parametrically driven and it is a good idea name it something logical like “Geometry before change on (today’s date)”. 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. This is sometimes very beneficial if the geometry becomes overdefined because it can be very challenging to repair an overdefined sketch.
14. Use the LogoPress 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.
15. 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.
16. Validate the sketch and there should now no longer be any errors in this punch.
17. Now, when you switch to the tool assembly, the tool assembly should automatically rebuild all punch cuts through all plates.
18. 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 rebuild without errors. If there are errors in the part files of the plates (usually cut features created when mounting a punch) then this may be just a rebuild issue. Open the part file for that plate and do a Ctrl+Q rebuild and the errored feature will most likely update properly.