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Thread: RV panel - importing Vans dxf drawing - Convert Entities

  1. #1

    Join Date
    Oct 2012
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    3

    RV panel - importing Vans dxf drawing - Convert Entities

    Hi all,

    I would like to model my control panel design in solidworks with a view to having the panel blank cut by waterjet based on my file. For those familiar with RVs, I have one of the deeper/wider RV-6 panel blanks with just the bottom flange pre-bent at 90 degrees to the panel face, so I need to cut the outer profile of the panel top and sides as well as the internal holes for instruments etc. Therefore, it is important that I have an accurate representation of the outside shape of the panel, which I should be able to get from the dxf file available from the Vansaircraft website

    I have now downloaded and opened this dxf file. As a complete Solidworks newbie who has just worked through some Youtube tutorials, I am advised that I have to "Convert Entities" from the dxf drawing into the Solidworks sketch I am currently editing. However, for some reason that I totally fail to understand, the application does not allow me to select the entities that I wish to convert. The "Entities to Convert" list box is open and highlighted but clicking on the various lines and arcs does not allow me select them.

    Can anybody spot the beginner mistake here?

    Loman

  2. #2

    Join Date
    Dec 2016
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    Zionsville, Indiana
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    Just open the DXF file and convert to SW objects.

    Once in SW, you need to fix some points or distances in the imported drawing. A you open the drawing, all the lines and dots will be blue. This indicates that these points can be moved. So you need to figure out what you don't want to change as you adapt the panel to the Bearhawk. Things like instrument cutouts, you can highlight and then FIX. That will mean all those points are fixed and won't change as you edit other features. I have been caught out a couple times by not being careful. Another way is to dimension the openings. Also establish the relationship between parallel lines

    I found that doing panel work in AutoCAD easier. You car down los a SolidWorks product, Draft Sight. It is fee software from Desault, the parent company or SolidWorks.
    Last edited by lathropdad; 08-05-2017 at 05:15 PM.

  3. #3
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Nov 2011
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    Israel
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    Hi Loman,
    I think I may have a solution for you - Can you post the DXF file here or if it's too big send it to my mail: jeff54il@yahoo.com.

    Jeffrey

  4. #4

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    Oct 2012
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    Hi Jeffrey,

    Any help you can provide is appreciated . It is a public file called F703X-1.zip on the Vansaircraft site but here is a link to my copy: (unzipped)

    I tried fixing all the required elements of the dxf drawing, as suggested by lathropdad, but I still get the same result with Convert Entities - can't select items. I think the problem may lie in identifying the plane and sketch into which I want to convert the entities. I am researching that line of enquiry just now

    I would prefer to persevere with Solidworks rather than go to Autocad or Draftsight as I want to work in 3D in order to produce cut-out/bend templates for items such as oil cooler shrouds made from flat sheet. I would also like to try out 3D printing. The panel project is a way of learning Solidworks but it is also an important element of my build.

    Loman

  5. #5
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Nov 2011
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    Israel
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    Hi Loman,
    OK - Got it.

    Short answer:
    Try File>Open>F703X-1.dfx>Open>Import to a new part as>2D Sketch>Next>Next>Finish
    Choose your favorite 3D part template (or the default).
    The part comes in as a 2D sketch on the Front Plane as a collection of circular arcs and straight lines, and unconstrained (blue) except for coincident endpoints.



    Slightly longer answer:.
    Now you have to decide what you want to do with the above. I will assume you want to add fully enclosed cutouts and perhaps edge cutouts that are not fully enclosed. i.e. you don't want to make a major change to the outer contour.
    3 ways to do this (there may be more):


    Method 1. Collectively pick all the graphic entities and then choose Fix - The sketch becomes fully constrained (black). You can do this now because you previously chose to import the dxf as a 2D sketch - not as 3D curves and not as "converted" curves. Now you can make any changes you want by deleting and adding geometry at your leisure.

    Method 2. If you want to retain the original dxf contour in the background and make a separate sketch for modification, then proceed as follows:
    Exit the sketch and change its name to something like "Original F703X-1" (The old name will probably be called (-) Model). Preselect the Front Plane, choose Sketch ​on the Front Plane (or any other parallel plane), choose Convert Entities, pick one of the contour curves, and make sure that the select chain checkbox is selected. Choose OK, and then go ahead with the changes that you need. For example:



    Method 3 (wild overkill, just a curiosity): After the 2D dxf import, Choose Tools>Dimensions>Fully Define Sketch>check Selected entities > collectively select all the geometry you need, and then Calculate. After a great deal of number-crunching you'll get much more than you need and the result will probably be of little use to you - a compendium of useless information. This is mostly an intellectual exercise, but it may be useful to know that the capability to automatically fully define the sketch exists in SW.

    Hope this helps.
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  6. #6

    Join Date
    Oct 2012
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    Thanks so much Jeffrey. That was a long and well researched answer and it has got me going at last. I used your method 2 and have also been able to expand the part so that the original top curved profile is applied to the wider and deeper RV6 extended panel blank that I will actually be water jet cutting to produce my final panel. I have since also managed to incorporate the strengthening flange that extends 1" back from the lower edge, perpendicular to the face, and applied accurate flanges to reflect the bend radius resulting from the way the blank was formed. From now on it is just a matter of sketching the various openings, arranging them and making extruded cuts with each sketch.

    I thought I had already posted my thanks but it seems I missed a step in that process also. Forgive my parent tardiness

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