View Scale in Multi-model drawings

[S_ACOSTA]

Normally I leave the view sacle as the drawing default, that way I can change the scale of all the views in one go, by doulbe clicking on a note tha has the &scale parameter in it.


My problem is that if I have a drawing with multiple 3d models, it only changes the scale of the views for the first model I placed in the drawing.


Is theresome workaround?


Thiswould be very usefull since the drawings can havecirca 50 parts, and typically you do not know how much space will be taken up until all the models have been brought in.


Thanks,


seb

 

[sumeet_k29]

Yes you are right Pro/e will change the scale of the model that was first placed on the drawing. Lets say you have two models A & B for which the views are placed. A is the model for which the view was placed first. Later on if you intend to change the scale of view for model B then you will have to go to Properties --> Drawing model --> set model and select the desired model and then change the scale of that.

 

[Dell_Boy]

If you run out of space, why don't you use the next biggest format size rather than change all the model scales?

If the parts are all common to a single assembly, is there any way of dimensioning them in a view of the assembly?


DB


Edited by: Dell_Boy

 

[S_ACOSTA]

Good suggestions, thanks.


The assembly a weldment, a little like a ship hull or one of those skeletons of dinosours.


I try to get the parts into a single drawing cause there are lots of them to be cut from a single sheet of metal, and also it is less work.


Also I can then export to DXF to have themplasma cut. The supplier prefers one drawing sheet with all parts same scale


Max printer sheet is A1, so when I get to that limit I mess with scales.


I did consider attempting an exploded view with all the parts on the same plane, but it gets difficult with all the parts, and I sometimes get a bug where the exploded state resets itself when I try editing.


It is not the end of the world, but would have been nice - and I was worried that I was missing some simple little trick/tweek.


Seb

 

[Dell_Boy]

You could always go up to A0 and just print it out at A1 if that is the biggest sheet your printer will handle. The dxf will probably need scaling any way.

Alternative solution. Create a special assembly with all the parts of interest laid out in a flat plane. Create a drawing of this special assembly. All parts will be at same scale that is easily adjusted.

DB

 

[dr_gallup]

Change the active model to the model you want to change the default drawing scale. You will see the scale in the lower left corner of the graphics screen. Doubel click on this and change it.

You will have to repeat this procedure for every model in your drawing.

 

[andysuth]

Can anyone change the scale parameter using relations?





I've got an automated drawing parameter change function I run through an MS Macro (combined with trail file) and I just can't see how to put a relation in the draft file to alter the &scale:0 parameter.





Any ideas?





I was thinking along the lines of an equation that was like:


ps=300


scale:0 =ps / MB_SPAN:4


Where ps is approx sheet width and MB_SPAN is a parameter from the assembly model.





Thanks,





-AS

 

[Mindripper]

I don't know the range of the sizes of the parts you are trying to include in a single drawing, but I suspect they vary significantly, so the use of a variety of view scales is inevitable on the drawing. But you seem to be thinking linearly in terms of your end result: providing geometry in the form of a DXF file to your fabrication shop containing all the parts at the same scale, for fabrication purposes.


My normal method of operation for getting a part madeis to provide a PDF file of the drawing and a DXF file of the part geometry ONLY at full scale. I export the drawing file as as a DWG or DXF from the solid modeling software, then open it in AutoCAD LT. In AutoCAD LT, I make sure it's full-scale and blow away all dimensions and the border etc., until only part geometry remains. Then I purge and save the file as DXF. The fabrication shop can then load the DXF file directly into their CAM software and simply pick the lines for cutter paths, etc. It sounds like you coulduse the same strategy, but I'm not sure if this can be done just within Pro/E. You may need a bonehead simplisitic 2D CAD program like AutoCAD LT for the DXF scaling and cleanup.

 

[andysuth]

Possibly not the best method when designing a crane though!