Greetings, all. First post.. I've just gotten started with SE2D (about ten hours of intense 'playing around'), and I haven't yet found a good way to do what I want. Basically, I want to have repeating elements at a particular radius at regular angular intervals. Say, 10 holes around a flange. All the holes are the same diameter, they're at every 36 degrees, and at the same radius. If the radius variable is changed, they should all move in (or out); if their diameter is changed, they should all change. I've managed to get something like this by drawing two radii at the appropriate angle, putting a hole at the intersection of the circle and one of the radii, mirroring it all around, and setting all the holes equal to each other, but then they can't be altered via the two variables. They look fine, as long as I don't need to tweak them further. There's the horizontal/vertical relationship; are there others that would help here? Thanks!
Here's a detail of part of the problem in the attached image. (In case it doesn't work, you can also see it at http://tinyurl.com/6fe2qj ) The dashed circle is the one around which the 'holes' should be spaced at ever N degrees; the dashed line is a radial I put in so I could place the hole. All the holes need to be the same size, and at the same radius. How can I make such placements more easily (without lots of temporary radials and mirroring), and tie them all to common variables for diameter and distance? So far my thwacking around in the bushes brings me up against 'conflicts with existing relationships.' Part two, and sort of related: The tiny circle has precise placement that I'm trying to automate, as well. It's centred on the radial, and a certain distance from the hole's centre. However, it also has a twin on the *other* side of the centre (now shown in the pic). Thw two of them need to be equidistant from the circle's centre; if one gets dragged farther out, the other needs to do likewise. Perfect for mirroring, but I can seem to get relationships going that say 'the centre is always on the radial' and 'the mirror point is at the intersection of the radial and the circle.' Trying to put in a hidden tangent line to mirror about also gets me the conflict message. A very cool tool, but I think I'm doing stuff more advanced than covered by the tutorials. :-) The whole bit of 'model,' 'drawing,' 'view,' 'geometry,' and so forth is new stuff to me; I'm used to just drawing on a sheet of paper. :-) Is there a good, complete, book (or other source) from which I can learn 2D in detail without worrying about 3D? Or is it all pretty much 'learn by doing and asking' ? Thanks!
Ken, Attached is a sample file, relationships.dft, for you to look at. It is a V20 file. I will try to explain some of the things I set up. It all works with relationships. Open the relationships.dft file. I have placed different geometry on different layers to help organize the display. Construction layer - Contains the construction circles and lines. Holes layer - Contains the holes. Driving dims layer - Contains the dimensions that drive the model. Driven dims layer - Contains the dimensiosn that are formula driven by the driving dimensions. The dimensions displayed are the dimensions that drive the model. Dimensions are variables. Variables can drive dimensions, so dimensions can drive other dimensions. You can define your own variables and formulas in Variable Table. You can also define a formula directly on a dimension. Click on Tools and then Variables at the top of the application window. This is the variable table. You can see all the dimensions and how they are defined. Close the variable table. Click on the 6.000 diameter dimension and change the value to 7.000. This dimension drives the smaller diameter construction circle. Notice that the larger construction circle also changes. This circle has a dimension that is defined to be equal to the smaller dimension + 1. The holes also move out with the change. Change the 1.5 diameter to 1.75. Notice that the larger hole circle changes. It is formula driven by the smaller hole circle. Change the 60 degree angle to 45 degrees. Notice that the spacing between all the holes change to 45 degrees. Click on The Layers tab to the far left in the edge bar. Click on Driven Dims layer and then click on the Show Layer button to turn on the display of the driven dimensions. Notice that some of the dimensions are green. These dimensions are driven dimensions. Right mouse click on the dimension for the larger construction circle. You will see Show All Values, Show All Names and Show All Formulas. There is also an Edit Formula. These allow you to change the dimension display and modify the formula on the dimension. You can also define a dimension formula by simply double clicking on the dimension. Double click on the dimension for the larger construction circle. You will see a Formula for this dimension "Driving_Dia + 1" without the quotation marks. Delete the text for the formula. Leave the formula definition field active. Click on the dimension for the smaller construction circle. The name of the dimension is added to the formula. Key-in "+ 1" without the quotation marks. You should see "Driving_Dia + 1". Press Enter to dismiss accept the formula definition. To simply set one dimension equal to another, double click on the dimension that needs the formula. Click on the dimension you want it equal to. Press Enter to accept the formula definition. Double click on the green dimensions to see how ther are defined. Also look at how the relationships are set up. If you have any questions about the example, please ask. Regards, Rick B.
Rick, your solution is elegant and very flexible, but shouldn't a simple bolt hole circle, as desired by Ken, be possible with the "bolt hole circle" tool? I ask this in part because I am unable to make this tool work. It just stops responding at the second instruction (either "click for the radius point" or "click for the second point" depending on the method chosen). Is this feature disabled in the 2D program? John Hilgenberg John Hilgenberg
John, The bolt hole circle command is an annotation command. It creates the circular centerline and center marks on an existing circular hole pattern. It does not create a circular hole pattern. Regards, Rick B.
Got it . . . Thanks. Let's put the circular pattern generator in the enhancement queue! John "Rick B." wrote: >John, >The bolt hole circle command is an annotation command. It creates the >circular centerline and center marks on an existing circular hole pattern. > >It does not create a circular hole pattern. > >Regards, >Rick B. > > John Hilgenberg