Drawing Templates/sizing issues? 1

[darnell]

Our company has been using SW since '97 but we are just now starting to use the drawing/templates part of SW. We have always did a saveas DWG and did the drawing work in AutoCad. My question is this;

When we start a new drawing in SW using a template we created of one of the title blocks, it comes in 1:1. If you change the scale to 1:2, the model gets smaller giving you the illusion that the border is now bigger. In SW, when you take a distance check, or add a dimension, everything is fine. At the same time, if you check the dimensions of the titleblock, they never change. If you do a saveas DWG and launch it in AutoCad, the titleblock is 1:1 and the model is now half the size.

We have always kept our objects 1 to 1 (full scale) in AutoCad and SW but why is SW backwards and not cross-Cad friendly when it comes to this?

What is a good work around as we will always have a need to tranfer back and forth to and from AutoCad?

Thanks in advance,

 

[badboggs]

I think what is really going on here is that you were really cheating in AutoCAD. You can't scale up the drawing format to fit the part or you are negating the size contraints on the format. A B size is 11x17 and you can't scale that. SW doesn't allow you to change the format size. That is why you have to scale the model. If you have to have the model at 1:1 scale then you have to use a larger or smaller template to make sure it fits onto the drawing correctly. That way when you import the drawing to AutoCAD it will be one to one.

So you will have to create a series of drawings

Ex. A, B, C, D.. ect..

Hope this makes sense.

Boggs

 

[darnell]

What we did in AutoCad was create a set of Titleblocks full scale or 1:1 in all the sizes (A,B,C and D). The objects are drawn full scale and the titleblock was inserted scaling it up or down around the object. You said you can't scale a B size 11x17, we did. We plotted to that scale. We also changed the LTscale and Dimscale so that everything looked ok. I thought this was standard practice moreso than scaling your objects like what is happening in SW.

 

[ctopher]

All parts should be always be created to 1/1 scale, then placed on to a drawing at a particular scale.

 

[Regg]

Although I never used Autocad, I always thought it (drawing in a scale of 1:1 and scaling the format) was backward from standard drafting. I am sure there were good reasons for doing this (possibly in the days of single precision you lost some accuracy if you drew at a scale other than one) Having done details and designs for many years before computer CAD programs, all you could do was draw in a scale if the part was to big for the paper you were using. And from my CADAM and Cadra days, these programs worked the same as SolidWorks. So for me, there is not much getting use to. As with any new software, you have to get use to the things it can do and hope there is an easy work around for the things (features found in other software programs) it cannot. Just so you know, I have my own gripes about SolidWorks but they, for the most part, are overshadowed by all the good things SolidWorks can do.

Regg

 

[ShaggyPE]

If you must saveas dwg or dxf, there is a check box under options to save 1 to 1 based on sheet size of view size. This will probably solve the export issue.

I use this feature when saving files that will be used on our cnc router table (wood shop). Prior to this feature being added (2001+) the cnc programmer had to scale the files I saved in order to get them back to the right size.

 

[badboggs]

Darnell,

If you actually scaled the title blocks and then printed to the correct size then the model would not be 1:1 on the print even though it was the right proportion. Though it would be 1:1 for the model. It really comes down to what makes sense. Most companies I've worked with don't even want a scale shown on the drawings. They don't want people to be able to take measurements from them. This simplifies worries about scaling errors.

Did we answer your question?

Boggs

 

[krywarick6]

Another way of looking at this is that SolidWorks handles things in an automated way that is similar to the paper space/model space function or tile mode in AutoCAD. The title block is always at 1:1 and the model is then scaled into the viewport. This type of cross over application is handle simultaneously in SolidWorks.

Christopher Zona
Litens Automotive Partnership
Concord, Ontario, Canada

 

[alexsasdad]

Step 1 Create a new drawing with no sheet format.

Step 2 Right click the drawing sheet and then click properties. Change the scale to 1:1. All drawing views should come in 1:1. If not change the scale of the drawing view to 1:1.

Step 3 Add drawing views

Step 4 Save as .dwg file

Hope this helps

Mike

 

[JNR]

I think the answer has been given. But just wanted to reiterate that SW is not being cross-CAD unfriendly. The basic premis of all (modern) CAD systems is the modelling is 1:1 (real world). Drafting is exactly that - just drafting. So if you have a 17x11 sheet - it is 17x11 period. All the text on it is 1:1 for a 17x11 sheet. The views of the models are scaled - just like in manual drafting. You didn't go get 50ft piece of paper to draw a car and write all the text 15" tall then photo reduce the whole thing to 17x11 did you? Unfortunately in the early days of multiple view for drafting purposes it was not as simple and it looks like you have inherited some older methods over the years in AutoCAD.

BTW: I am not at all unsympathetic with your legacy dilemma. I am painfully aware of the old issues of "draw scale/plot scale" etc. (CV CADDS3 anyone? - yeah, I go back aways.)

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