Back To 2D1 Dec, 2000 By: John E. Wilson
Even though transferring data directly from computer 3D models to the machines that manufacture parts is becoming increasingly common, you often still need to make fully dimensioned multiview 2D drawings from your 3D solid models. AutoCAD has a set of tools for transforming its solid models into 2D drawings, and this months 3D column will describe those tools and explain how to use them.
The Trouble with Solids
A logical approach toward creating a 2D multiview drawing from an AutoCAD 3D solid model would seem to be to first set up Paper Space floating viewports having orthographic-type viewing directions, and then add dimensions to the model in those views. However, there are problems with this approach.
You cant show hidden edges on solids as dashed lines. They are either not displayed at all (in hidden-line removal viewing modes), or else they are displayed in the same linetype as visible edges (in wireframe viewing modes).
No direct and practical way exists to create section views.
Even though the edges on a solid may look like lines, arcs and circles, they are not, and AutoCAD dimensions do not work properly with edges. Furthermore, edges are likely to be directly on top of other edges in orthographic views, which complicates object selection.
A better approach to making 2D drawings from 3D solid models is to project the models edges and profile onto a plane where they are drawn as 2D objects. AutoCAD has three commands for doing this: SOLPROF, SOLVIEW and SOLDRAW. SOLPROF is for making drawings with pictorial views, while SOLVIEW and SOLDRAW are used in tandem to make multiview orthographic drawings.
AutoCADs SOLPROF command projects the edges and the profile of a selected 3D solid onto a plane that is perpendicular to the viewing direction. It is especially useful for creating the axonometric views, such as isometric views, commonly used in catalogs and parts manuals. The projected objects are in an anonymous AutoCAD block (one that has no name) for easy management. The four steps to create such views in AutoCAD 2000 are:
- Select an unused Paper Space layout by clicking its tab, and use the PAGESETUP command to choose a printer and a paper size.
- Use MVIEW or VPORTS to create one or more floating viewports having a size of your choice. Depending on the settings in the Display tab of the OPTIONS command, AutoCAD may automatically create one viewport for you. You can use this viewport if you like, and you can stretch it into the size you want.
- Go into each viewport with MSPACE (or simply double click within a viewport), and establish the zoom level and viewing direction you want.
- While you are still within the viewport, invoke SOLPROF and respond to the commands three yes-and-no options. The first of these options allows you to specify that hidden edges be placed in one block and visible edges in another. In most cases, you should accept this option. If you accept the second option, SOLPROF creates a 3D wireframe from the edges of the solid, rather than making a 2D projection. Such a wireframe is not likely to be useful in creating a 2D drawing. The third option determines whether or not tangential edges will be displayed in the profile. Tangential edges represent the points of tangency between two adjacent surfaces, such as between a fillet and its adjacent faces.
Figure 1. AutoCAD's SOLPROF command makes axonometric drawings from AutoCAD 3D solid models by projecting the edges and the profile of the model onto a plane perpendicular to the viewing direction.
The Roles of SOLVIEW and SOLDRAW
Although you could use SOLPROF to make multiview 2D drawings from 3D solids, SOLVIEW and SOLDRAW are intended exclusively for that purpose and require much less work on your part. SOLVIEW sets up views of a 3D solid model in Paper Space floating viewports, and SOLDRAW draws 2D objects suitable for dimensioning in those viewports. These two commands also tie the 2D drawing closer to the 3D model than SOLPROF. After making a drawing with SOLVIEW and SOLDRAW, you can change the 3D model, rerun SOLDRAW and the changes will be reflected in the 2D drawing.
You create the SOLVIEW viewports one at a time by specifying the type of viewUCS, Ortho, Auxiliary or Sectionfrom a command-line prompt.
Figure 2. AutoCAD's SOLVIEW command sets up Paper Space floating viewports for making a multiview 2D drawing from a 3D solid model. After establishing a base view, you can create views othogonal to it and also create auxillary and section views. The SOLDRW command draws 2D representations of the model in these viewports.
SOLVIEWs Ortho option makes a view that is folded 90 degrees from an existing view. A command-line prompt will ask you to establish the viewing direction by picking a point on one side of the base viewports border. AutoCAD will lock into the ortho mode, extend a rubberband line from the border and prompt for the center of the new viewport. Then you will set the size of the new viewport by picking points for two opposite corners. The final prompt of this option asks you to assign a name to the viewports view. You will not be prompted for the viewports scale because it will use the scale of the base viewport.
The Auxiliary option creates a viewport having a viewing direction perpendicular to a plane seen edge-on in a base viewport. It is useful for showing true sizes and shapes on a plane not aligned with any of the principal planes. You will be prompted to specify the plane by picking two points on its edge in the base view and to specify a direction for viewing the plane. AutoCAD will rotate the Paper Space UCS so that its x axis is perpendicular to the inclined plane, anchor a rubberband line on the plane, lock into the ortho mode and prompt for the auxiliary viewports center. When you have established the center of the viewport, you will pick two points for its opposite corners and give its view a name. The auxiliary view takes the scale of the base viewport.
The section option of SOLVIEW sets up a cross-section view that slices completely through the model. You will be prompted to establish the edge of the cutting plane by selecting two points in a base view and a third point to indicate the side from which the section is to be seen. SOLVIEW will anchor a rubberband line on the cutting plane, activate the ortho mode, prompt for the center of the section views viewport and prompt for two points to establish the size of the viewport. You can assign a scale to section views different from the base view. The last prompt of this option is for the views name.
SOLVIEW doesnt draw anything other than floating viewport borders; it does though, create special layers used by SOLDRAW for drawing objects in the viewports. These special layers are for visible objects, hidden objects and hatches (for section views only). The layers for hidden objects use AutoCADs HIDDEN linetype, if it is loaded. SOLVIEW also creates, as a convenience for the user, layers for the dimensions. The names of these layers are based on the names you assigned to the viewport views and layers are selectively frozen so that objects appear only in the proper viewport. For instance, if you assigned the name TOP to the base view, the visible objects in that view will be in a layer named TOP-VIS, and that layer will be frozen in all of the other viewports. SOLVIEW puts the viewport borders in a layer named VPORTS.
When you have your drawing views established, you will exit SOLVIEW and move on to SOLDRAW. SOLDRAW is a command requiring little user input, but it does a great deal of work. You simply pick the Paper Space floating viewports made by SOLVIEW, and then sit back and watch as SOLDRAW goes about drawing objects in those viewports. When it is finished, the 3D solid model is no longer shown. In its place each viewport contains a 2D drawing of the appropriate view of the model. If there are section views, the sliced areas will be hatched. All of the objects in the 2D drawing views are within Model Space.
The Nine Steps to Making a 2D Drawing
- Decide on the drawing views necessary for completely defining the part, the size of paper the drawing will be printed on and the scale of the views. This is a step you would do in setting up any 2D drawing, whether directly on paper or with a computer.
- Open the drawing file containing the 3D solid model. Load the HIDDEN line type, so that AutoCAD will use it for the layers it will make for hidden objects.
- Select an unused Paper Space layout by clicking its tab, and use PAGESETUP to select a printer and a paper size corresponding to the one you selected in Step 1. Be certain that the Paper Space scale is one-to-one. (Remember: Paper Space scale sets the relative size of objects that are within Paper Spacenot within the viewports.) If AutoCAD has automatically created a floating viewport, erase it.
- Draw or insert a border and title block for your drawing. Although some people postpone this step until dimensions have been added to the drawing, most find the border and title block useful in judging the locations of views when they are using SOLVIEW.
- Start the SOLVIEW command. Use its UCS option to make the base view of the drawing. Often this will be the top view, but it doesnt have to be. Then make the drawings other views. You can make them all during one call to SOLVIEW, or you can invoke the command several times. The size of the viewports is not critical since you can later make them larger or smaller, if the need arises.
- Save your drawing file. Start the SOLDRAW command and select the floating viewports created by SOLVIEW as the viewports to be drawn.
- Set the colors of the layers SOLVIEW created so that they meet your standards, and also set the dimension parameters to your standards. The dimension parameters will be the same as for a 2D drawing, except for dimscale. You should set dimscale to zero, either directly or by checking the Scale dimensions to layout (Paper Space) button in the Fit tab of DDIMs dialog box. When dimscale is set to zero, AutoCAD automatically uses a value matching the zoom level of the viewport in which dimensions are being added.
- Add dimensions to the drawing views. This one step will take more time than
the previous seven steps. You will add dimensions within Model Space, working in
one floating viewport at a time, using the following procedure:
**Zoom in to get a good view of the viewport you are going to work with. Use the MSPACE command, in any of its several forms, to switch from Paper Space to Model Space, and click within the viewport you intend to work in to make it the current viewport.
**Use the View option of the UCS command to orient the x and y axes to match the view. Follow this with the Origin option of the UCS command, and use an object snap on some object within the viewport. This will ensure that the dimensions will be on the same plane as the objects being dimensioned.
**Set the layer for the dimensions to match the view. For example, if the view in the viewport you are working in is named TOP, select the layer named DIM-TOP. This will cause dimensions to appear only in the proper viewport.
**Add the dimensions as you would in any 2D drawing. If the viewport is too small to accommodate some dimensions, temporarily switch back to Paper Space and stretch the viewports border. Do not zoom or pan within a floating
viewport. (An option in the VPORTS and MVIEW commands allows you to disable zooms and pans in selected floating viewports.)
Figure 3. This completed 2D drawing is based on the viewpoints shown in figure 2. As with any 2D drawing, you must manually add the dimensions.
- If necessary, move the views to better fit the paper and borders you are using. While you can freely move viewports and change their size, you must make certain you do not alter their scale or their alignment. When the views are as you want them, turn off or freeze the layer named VPORTS. The drawing is now done. Figure 3 shows an example.
Limitations and a Glitch
The SOLVIEW/SOLDRAW command combination is a quick and easy way for you to transform a 3D solid model into a 2D drawing, but it does have some limitations. You cant create offset or partial section views, partial auxiliary views or detail views that have a scale different from the base view. Moreover, tangent edges are never displayed, which may cause the part to be incompletely delineated. SOLPROF is able to display tangent edges, but it sometimes has problems with them, as you can see by looking closely at Figure 1.
Dimensioning is more complicated than it is in most pure 2D drawings because you must add dimensions on a view-by-view basis in Model Space and use a layer thawed only in the appropriate viewport. The alternative of adding dimensioning in Paper Space is not practical because AutoCAD does not fully recognize Model Space objects from Paper Space.
You will encounter a SOLVIEW glitch if you attempt to use multiple layouts. You will recall that the purpose of the Paper Space layouts introduced in AutoCAD 2000 is to permit you to have multiple drawings within a single file. You can, for example, have a D-sized fully dimensioned drawing for manufacturing in one layout and a simplified A-sized drawing for marketing in another. However, when you use SOLVIEW to create viewports in a second layout, AutoCAD creates extra layers with names based on handles, similar to those created by SOLPROF, and assigns those layers to objects that should be in the SOLVIEW layers for visible and hidden objects. This bug severely impacts your use of SOLVIEW in creating a 2D drawing in a second layout.
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