设计库-自动缩放fe

shift1313 · 发表于 2022-7-9 07:19:45

嘿，特洛伊，我想出了一个办法，但有一个轻微的转折。我会尽力解释的。

首先，我画了一个50x200x15mm的矩形板。大小其实并不重要。

其次，我创建了一个参考草图。如果你看附上的图片，你可以看到它。那个草图是我的盘子两端偏移50mm，然后是这些线中点之间的一条直线。

第三，我在一个新草图中创建了一个15mm的圆，并将其挤出切割为10mm。

第四，我创建了一个矩形，由第二步的偏移端组成，然后转换15mm孔的边缘并修剪所有东西。我偏移参考边的原因是，我不必指定槽的长度。假设这个盘子是50毫米宽，但你想把它用在一个100毫米宽的盘子上，这仍然有效。

第五，我使用步骤2中中点之间的水平线创建了一个曲线驱动的图案。确保选择等间距。

创建所有这些特征后，可以打开设计库（并将其固定打开），然后按ctrl键将两个挤出和曲线驱动图案选择到所需的特征库中（新文件夹）。

创建新零件时，需要绘制板，然后绘制与我在步骤2中绘制的相同的参考草图。将特征拖动到零件上时，需要选择第一个孔的中心点，即50mm的偏移边，以便定义槽，然后选择中点之间的线来定义曲线驱动图案。

现在你需要做的是创建其中的几个特性（这不会花费任何时间）。您将需要一个3键孔特征、4键孔特征等等。另一个选项是，将此特征插入新零件后，在特征树中展开特征库零件，并更改曲线驱动阵列中的特征数。这不应更改设计库功能，只要您在树中单击功能时不将功能另存为sldlfp，则数字应显示在模型上，并将进行快速编辑。我还没有想出在特征创建期间输入数字的方法，但我认为这是一种相当有效的方法。

pawsche · 发表于 2022-7-9 07:22:09

嘿，马特，

再次感谢您的回复。

非常好的说明。当我把它插入一个新的零件时，我完全按照你所说的做了，我需要定义第一个孔和水平线段的起点。

按照我在第一篇文章中所做的方式，我所需要做的就是点击基线、两条边（零件的左侧和右侧）和零件的顶行，它为我做到了这一点。这意味着我不需要插入任何行或任何东西，因为这四行已经存在，这很容易

pawsche · 发表于 2022-7-9 07:25:40

Hi Matt,

Me again . Sorry for more questions. But just curious.

If that reference line was always 24mm above the base and always 50mm from the side edges of the part. Is there anyway to make solidworks ask for the base and the two side edges when you insert the feature (instead of the reference line) ??

Or does it request that line instead because its used by the curve pattern.

Thanks again,
Troy

shift1313 · 发表于 2022-7-9 07:29:18

Hey troy. What is asked of you when you insert your feature from the library all depends on how you created the feature in the original part. In my example I used reference points/line to locate everything. If you located your first feature with a 50mm and 24mm dimension then it would require you reference edges to locate your part. Same thing, if you used a midpoint reference to create your sketches, then it will ask you for that. If you gave no reference(under defined sketch) it would not ask for it. I try to use converted enties, offsets and reference lines because the geometry updates based on your base part. If you need it to be 24mm from the edge every time then you can either give the curve for the pattern a 24mm dimension(not at the midpoint) or choose to define the entire feature another way.

The main reason I used the reference line was so my curve driven pattern had the length of the line. Offsetting the edges ensured that not only were they always 50mm off the edge, but that my curve driven pattern was based off a reference line between those so it always updates properly.

The main difference between the method I used and the one in your original post I think is that you did your array inside the sketch right rather than as a feature? Doing it as a feature allows you to easily adjust the number of features without entering a sketch or editing the feature. This is why I chose that route because you mentioned some times its 3 holes, some times 4 or more.

Ill try to work up another example that may be more suited towards what you are doing.

shift1313 · 发表于 2022-7-9 07:33:59

Troy I played with it a little bit over lunch and I am not seeing an easy way to do this keeping the ability to change it from 3 features to 4 and so on. Doing it in a sketch as you did will allow you to pick just the edges as reference but you loose the ability to change the number of features easily. Doing it by creating the refence sketch as I did takes a little setup but allows easy change of the number.

Ill have to think on it a bit more when i get the chance. Is the number of features always 3 or 4 or can it be any?

pawsche · 发表于 2022-7-9 07:37:10

Hey Matt,

Thanks again for all your help and explanations. I think your technique is the way it should be done as you can change number of instances really easy, I have been playing with it .

The designs I use typically only have 2,3,4 cam holes. And I have done library parts for all of them and have included 5,6 with your curve driven technique. It works perfect.

Yes I did that geometry thing in the sketch where I defined the location of the 15mm holes.

Cheers
Troy

shift1313 · 发表于 2022-7-9 07:39:21

Glad you have a solution that will work for you troy, and thanks for the question. I enjoy thinking about these types of problems. I really havent dont much with design library features besides forming tools for sheet metal parts so it was fun:) Ill keep thinking about it and if i come up with any other solutions Ill be sure to post them here:)

pawsche · 发表于 2022-7-9 07:43:48

Thanks Matt really appreciate your time.

No need spend more time on it Matt, I have all I need now 2,3,4,5,6 have done a set for vertical and horizontal edges its so cool

shift1313 · 发表于 2022-7-9 07:45:01

When you insert your design feature if you drag it around your part it should correct itself. Look at the pop up image showing you what edges its looking for. If when you place it you are closer to one edge and you make your correct selections I dont think you would need a different one for vertical/horizontal. Im not at SW so i dont know that for sure, but i think thats how it works.

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