Jump to content

Accurate drawing for CNC cutting

Recommended Posts



Does anyone still use VW for drawing things which need manufacturing with any degree of accuracy? For example, metalwork which needs CNC cutting on a mill, laser or waterjet?


I find that VW's 3D modelling is generally great but extracting geometry for real-world machining is like having teeth pulled. 10 times as complicated and not entirely accurate.


Even though objects are drawn by numbers to a precise size, when it comes to dimensioning a viewport, VW seems to be only somewhat accurate. It's almost always a decimal point or two out. And when it comes to actually making a DXF file to send out for production, the drawing has to be almost always done again in 2D because arcs become beziers, arcs are split and circles become semi-circles etc.


Snapping seems also to have become a bit vague and I find myself deconstructing models and realigning objects over time in spite of rigorously aligning them in the first place.


Or is this just me?


Link to comment

Have done a lot of such work. The problem is often in the other end, that is, many of the programs used for controlling CNC machines have severe limitations. The software is often simplistic and often ageing. I therefore suggest keeping geometries on a very basic level. In 2D, it typically means using lines, polygons, and arcs to define things. Avoid Berzier and spline curves. Avoid symbols and groups. Avoid using filled surfaces, and for example using Clip Surface to define a hole in a closed polygon/polyline shape. On polylines, only define shapes using straight lines and arcs. 

  • Like 3
Link to comment

I often use Vectorworks for CNC router and waterjet and laser.  The files are exported to dwg for through cuts, dado/channels and some surface "tattoo".  All this is for flat material - steel, stone, glass, plywood, plastics . . . almost any sheet goods with parts made to bow/snap together or fasten with bolts, screws, dowels, tab/slot.


My workflow is usually a parallel 2d/3d. I could probably use autohybrids, but prefer to have separate design layers for 2d and 3d.


Heavy use of symbols -- 1/2" bolt hole? that's a 2d symbol. It can be altered throughout to compensate for fit parameters.


I also use color schemes which are consistent 2d and 3d. eg every instance of Part #6 is light blue in both 2d and 3d.  Other parts do not have this color.


As for precision, I have no trouble with snaps.  I agree with all the advice from @Claes Lundstrom :

  • Stick with straight lines and arcs.  The older cutting software may not correctly follow a bez or spline path.  But, you can test this with the cutter early in your design phase.  Some of the newer router software has no trouble.  Also conversion to dxf/dwg can mess with things, especially older versions.
  • Round holes in a perimeter shape - Don't clip surface the 2d perimeter. That process converts the circle into a polyline. Use a "floating" circle.  Underlaying guide objects can assure centering.
  • Precision - Note that waterjet introduces drafting to the edge.  The jet gets turbulent and looses energy as it progresses into the depth and along the path.  Bottom of cut is narrower than top.  eg the bolt will not pass, or the perimeter shape will not fit into the target slot. Kerfing sets the jet to appropriate side of the path, but does not necessarily compensate for the drafting. Compensate as needed during design with offsets. You can ask the cutter to make fit tests for you. Or have all compensation done by the cutter. But that can introduce changes you might not appreciate. I don't like others altering my drawings.  Ask for a spec on the draft and make your drawing conform.
  • Nesting - I can always beat the nesting software.  Just allow for kerf and some buffer.  Work out nesting parameters with the cutter.  Note that many waterjet services can run dual or multiple nozzles eg offset by sheet width so that a single nest on one sheet can cut two sheets simultaneously  and produce double the parts in one go -  saves cutting time and $.  Lasers and routers can probably operate multiple cutters as well, but I have no experience with that.
  • At end of design, paste a copy of the 2d elements into a separate cutting file containing a single design layer - no sheet layers, either.  Then convert all symbols to groups, ungroup all groups.  Might mean multiple applications of Convert to Group and Ungroup so that everything is simple vectors rather than container objects.
  • Convert the vwx cutting file into a dwg/dxf. Choose the most recent rev the cutter can use.
  • Also create a pdf for paper print to show your intended parts or nest of parts in scale.

Develop a good working relationship with the cutting folks.  The workload and errors will drop dramatically as you each start to understand the needs of the other.


OK, lots more to this but the above should help at the start.





Edited by Benson Shaw
Never ending details. Never get 'em all
  • Like 2
Link to comment

Thanks for the replies.


We own our own CNC machines from multi axis mills and turning centres to flatbed routers, some with Siemens controllers (mainly dreadful) and others with other controllers and software so I know well the limitations with post-processing VW DXF files for CNC.


For production parts, I only do use lines, arcs and circles. However it's the VW surface extract tool which converts arcs in polylines to beziers, not me! Useful entities like rounded rectangles (for a machined slot) are converted into a mess of points. I have to go back and either redraw or manually extract the original arcs and lines profile from the model and paste it into the 2D file. Is this what we use CAD for? Not me!


You suggest doing a paper PDF print… it's this which is the major time sink. You might accurately draw a shaft or a bore in VW to 1" but when you come to dimension this in a viewport, VW will rarely give you an even number like 1.00 any more, it's aways inaccurately to one or two decimal places which of course is useless for production of anything other than cheese. And trying to extract a diameter from a circle doesn't seem to work at all unless you draw the circle again in the viewport annotation. All this leads to mistakes and a loss of precision which oddly, is what we started using CAD to avoid. You should not have to draw a part twice.


I had a Morgan Plus 8 once. Morgan specified the length of the car to ±2"! You would not get away with that any more. But as they said to a parliamentary enquiry, "We have a five year full order book, and you?"


Post processing software varies enormously. One program takes groups but insists on the outlines of polys being decomposed. Another won't see a group but is OK with contiguous polys. You learn this. For work done outside, we normally take the dumbest option.


However, it's for outside work that we get the most problems where either their post-processing software is different to that which we use, or more usually, the operator doesn't know enough about CAD to run it or they require drawings to an accuracy which VW seems unable to offer without a lot of workarounds.  


In most cases, in-house, we decide in the post processing software how to sort the paths because it's a tool path then, not a drawing. So with round holes in a perimeter, what we do is based on the tools used to cut the shape.  Most of this is tedious but well understood. 


"Nesting - I can always beat the nesting software" You're using the wrong software! I've been nesting since MiniCAD 4 and I would bet you that there isn't a human out there who can do better than the best nesting software unless the shapes are simple and/or the time really long. As a test, I have nested really complex toy puzzles in 10 seconds which would take almost anyone minutes to complete. I have nested files with hundreds of shapes over 3000 feet long down to a fifth of this in under 20 seconds and got results which were 5% better than I could achieve in hours.



Link to comment


Ahh - You have loads of experience and major equipment in house. Didn't see that from your initial post. My remarks above and here are aimed more at those exploring CNC with external cutting services.  


I hope you will add your knowledge to future questions on these forums.  Lots more vwx operators are embracing CNC work and come here for help.



  • 3d to 2d - That problem with loss of 2d primitives when extracting from 3d is not something I have solved directly. I have a hybrid workflow which does not fail at dimensional control.  It's almost always for sheet goods, so zero experience with the 3d milling, and only minimal experience with variable z router control and shifting the attack angle of waterjet. My 2d symbols are created and nested on a dedicated design layer. 3d symbols directly overlay the 2d symbols on a separate layer and are developed as extrudes, solid subs, etc from primitives in the 2d symbols. The 3d assembly is formed on yet another layer. Edits to the 3d instances in the assembly translate to the 3d instances on the nest layer. Edit in the 2d nest by matching to the overlaying 3d. That's the basics, anyway.  Sorry, not worlds most efficient flow, but eliminates many problems working with the cutting services.  They tell me my files are super clean and need only path verify plus their kerfing and tabbing.
  • pdf - This is not needed at all for your in house processing, as whole team sees same paths via same software.  I recommend pdf as a way to indicate for the cutter the intended layout and part count. Colors or line types can distinguish parts from drops.  Cutter can respond with a pdf proof of the cut paths. Overlay my pdf verifies whether the dwg export was interpreted correctly.
  • Nesting - I don't own or use any nesting software. Apparently I can at least beat nesting proposals I received from cutter's ancient nesting software.  I send out for cutting only occasionally and my part count per sheet is usually under 100.  Time commitment is not great.  So, I retract the boast that I can always beat it.  Good call!




Link to comment
10 hours ago, DMcD said:

For production parts, I only do use lines, arcs and circles. However it's the VW surface extract tool which converts arcs in polylines to beziers, not me! Useful entities like rounded rectangles (for a machined slot) are converted into a mess of points. I have to go back and either redraw or manually extract the original arcs and lines profile from the model and paste it into the 2D file. Is this what we use CAD for? Not me!



I agree that it would be very useful to be able to control the number of points (beyond high, medium and low), and exact behaviour of a given curve. In my main 3D modelling program, I can set it locally for each given element, part of an element, and numerically to whatever I find relevant for any given task.  I find it extremely useful, and could probably not live without it for my type of work. 

  • Like 2
Link to comment

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.

Reply to this topic...

×   Pasted as rich text.   Restore formatting

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

  • Create New...