Need help scaling down a model

Will someone please help me in my dumbness. Not all that long ago, I
made a model of a blanking die, 4 X the actual size that I needed. I
now need it of course 4 X smaller and I cannot reduce by 4X, only
enlarge by 4X. I am assuming that the parameters would be 4:1 to
enlarge, and 1:4 to diminish? I am missing something basic here in the
technique, and I really would appreciate someone reacting to this plea
with a step by step on the sequence required to diminish. I am using
SWX 2007.
Love this forum, by the way, I have learned so much from you guys,
that I feel guilty not being at a level that I can contribute. Yet,
anyway.
Thanks in advance,
Amy Labritto
Reply to
amylabritto
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In the part model, Insert>Features>scale enter value of .25
Note that none of the model dimensions will imported (insert>model items) into the drawing will show this scaled down model (you will have to use driven dims created in the drawing) Ed
Reply to
Edward T Eaton
Amy,
Ed made an assumption that the model in question is only a part file, and did sort of state that assumption, but you may not have caught it. If it's an assy, then things are not quite as simple in that the scale feature only works on parts, so you would have to scale each part individually and then make any necessary adjustments in the assy to put things back where they belong.
If your model is in fact just a part file, then great. If not, then I didn't want you to get frustrated because you couldn't get it to work.
By the way - why did you originally model it 4x too large?
WT
Reply to
Wayne Tiffany
Well that is a comedy of errors in and of itself. It is a profile line drawing of a very complicated nature, (multi electronic contacts), and the Pantograph Engraver needed a printout exactly 4 times the actual size so that he could engrave a master pattern for the Pantograph, and then he could use that 4 times larger pattern, set his ratio at 4, and engrave right through a thin piece of Berillium Copper, (.017"), with a small faced cutter to make an extremely clean and accurate profile of the blank needed to make the prototype, that needed to be drawn up and bent at all sorts of angles, tiny small diameter rolled contacts, male fork types etc, etc. I had issues, at that time, with my version of Autocad, (14, I think), in that the plotting section had a bug in it that would not allow me to plot in ratio, but it would allow me to plot 1 to 1. What was laughable about this, is the fact that because of the way we went about making the prototype, the client put the finished prototype under the scrutiny of a shadowgraph, saw the high quality, and he actually accused us of having the tool allready built and were charging him for a tool that we had in inventory. It's a case where this company was literally punished for seeking perfection in a prototype, which this company is known for, and enjoys the appropriate reputation. Thank you Mr Eaton, and thank you Mr Tiffany. Amy Labritto
Reply to
amylabritto
Try working with design table and and use equation to define various dimensions. I wish then u will able to make configurations and hopw this will do the job as per ur requirements. Even also add relations of dimensions in the assy mode so that u don't have to change many parameters.
regards
Deepak
Reply to
Engineer
Amy,
The way I read your explanation of what happened, is your strip layout is 4X size, but the rest of your tool is modeled to the correct size, albeit designed to an oversized strip layout.
Do you need to do is get your strip layout to the correct size? There are several ways to correct your problems, but the exact answers depend greatly on how you created your models; ie, how much in context stuff, etc. What is the master for your design, the strip layout I assume. You will need to use a combination of techniques, I suspect.
You may not be able to just scale your parts down. What about holes, dowels and fasteners.. are those 4X to big? The guidance system for the die asm, are the guide posts to big or just in the wrong locations because your die shoes and major die components are oversized in the plan view of the tool. What about your shut height for the tool is that 4X to big? Do you see where I am heading with my questions. The scale feature will only help you to a point.
If I am reading what your issues are correctly you have a big problem and there will be no magic bullet for you. Personally, I would be considering starting a new assembly and building it correctly. If you have to live with the tool design for any length of time you will always be annoyed to have to work on it because it is messed up. If you are sending this math data and drawings out to someone else to build, I would not want my name on the models for anyone else to see.
Wish I could offer you an easy answer, but I think you are going to need to bit the bullet and make it right and chalk up your error to a big learning experience that you will probably remember for a very long time.
Regards,
Anna Wood
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Reply to
Anna Wood
I have the same problem as Amy, except I have to deal with a 100-some part assembly.
The assembly is made of almost all imported geometry, and none of it lines up with orthogonal faces. It's all basically just fixed in space. Somehow it is now 62-some percent too large. Is there anyway I can make this thing into one big "part" (I don't mind losing all of my subassemblies) with multiple solids? Then I could scale the stupid thing, then go back to an assembly.
Thanks + any other ideas?
Reply to
lipkink
Sure, just "Save As" and pick "Part" in "Save as type:". Check the "All components" under "Assembly geometry to save in part file:".
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
Reply to
Jerry Steiger

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