Create a new tool from a previously created tool

Of course one of the most powerful things about CAD has always been the ability to reuse data. LogoPress has a very powerful command called “Save as… with new project name“.

First of all, note that when you start a new tool in LogoPress, it includes the ability to create a “project name” for this new tool. In doing so it automatically includes this project name in all parts that get inserted into the tool so you don’t have to worry about problems with commonly named parts. Avoiding commonly named parts is an important consideration when working with any parametric software. This automatic project naming is a great feature and a major time saver. It also eliminates a lot of headaches that can occur when doing something like this manually in SolidWorks, or worse yet, when not doing it at all.

This LogoPress “Save as… with new project name“ command could be used right after finishing a design if the next design will be very similar, or it could be used months or years after you’ve finished a design. Perhaps you receive a new order for a die that is very similar to one you’ve done in the past. So, with your old tool open you simply do a “Save as… with new project name” (found under the LogoPress pull down menu) and LogoPress will create a completely new set of files that is identical to the previous set (including drawings) other than the new project name of course. It will, of course, break all references to the original project. This is done in a matter of seconds – depending of course on hard drive speed and the size of the tool.

After using this command, you typically have two different methods for working with the newly saved/created project.

1. If there is a relatively big difference between the old part that was in the previous project and the new part that will be in this newly created project, you would use this first method. - You would delete all strip related items that are in the tool, starting with the punch mounting hardware, then the mounted punches themselves – usually by using the LogoPress “Delete punch” function, and then any cavities that have been cut for said punches (this happens automatically when using the LogoPress “Delete punch” function), and ultimately deleting the strip assembly itself, including the part that the die was originally created to make. You would then create and insert a completely new strip into this tool that was newly created tool.
2. This second method would get used if there was a relatively small change being made to the part that the new die is getting created for. You can keep the existing strip and rename the part so that it is now named with the new part name/number. This method maximizes the reuse of data benefit.

The rest of this post will focus on the specific instructions for using the second method. Please follow these steps carefully. As a reminder, the “Reference part” is the part that you are designing the die for. It is what the strip and the tool revolve around, so to speak, and it is the one part in the strip and tool that does not get a project number. The “Annex part” is the part whose name always ends with “_for_strip”.

1. Open the strip assembly that contains the new project number
2. Open the old reference part (note that the reference part (the part that the die will be making) is the one part in the tool that does not get a project number)
3. Rename the reference part to the new name using the SolidWorks “Save As…” command. When you do this, do NOT check the “Save as copy” option. (If, when using this “Save As… ” command, you get a SolidWorks dialog box that pops up with a warning about the “Save As” command and replacing references, click OK. Optionally, if you are a more advanced user and you understand what this dialog box is telling you, you can check the box that says “Don’t ask me again”)
4. With this newly named (via the Save As command) reference part open, press CTRL+Q to force a rebuild. This will create new body files with new names referencing this new reference part name
5. Open the annex part that is in the strip assembly and rename it using the SolidWorks “Save As…” command (again, do NOT check the “Save as copy” option) being careful to note that the project name/number should not change
6. With this newly named annex part open, edit the first feature in the tree , that is the LogoPress “Import” feature and browse to select the newly named reference part name, then check okay to validate
7. While in either the annex part or the strip assembly, on the LogoPress pull down menu, select “Update the stations of the Annex part used in the strip“
8. For the sake of housekeeping, I suggest you navigate to the folder containing the old parts that are now unused in this new project and delete these old parts – the old reference part, old annex part and old body files
9. Now you are free to make changes to the new reference part as needed to reflect the difference between this new part name/number and the old one. Don’t forget to press CTRL+Q to rebuild the body files and after doing so of course, you will need to use the “Update the stations of the Annex part used in the strip” command again.