I use drawing to export DXF files.
I want the edges of my part to align with the sheet edges.
Not just close, but dead-on control of a view location.
What is you end need with that?
I need zero-zero of the DXF to be in a specific location. I also need the duplicate line removal of the drawing to get a clean output for several post processes. Eyeballing just proved disastrous (days lost!).
I can easily do this in PTC Creo. I need a way to duplicate this in SW.
We have the same requirements here as well.
Our WireEDM department needs to move the DXF geometry so the "pick-up" location of the block (sometimes 2 edges, sometimes a specific hole) coincides with the 0-0 of the machine. In MasterCam they can move the geometry, but it is not always quick or easy. Additionally, I can convey my design intent (what to pick-up) to the Wire guys if I move the geometry (intended pickup position) to the home (0-0) position. The pick-up location (for WireEDM) is often (almost always) different from the zero-zero edges of the block.
Also, and this is a BIG problem, we MUST remove duplicate geometry. The WireEDM scrapes the block whenever a duplicate round hole is present and not removed.
Our only solution to solve both problems is to save as DXF from SW and import into KeyCreator. In KeyCreator it is a simple and easy task to run a macro that moves the geometry from a selected location to 0-0-0 and run a "Compress Curves" function that remover all duplicate entities and moves all geometry to the Z-zero plane. We also conveniently change the colors of the geometry to the desires of the Wire guys for best contrast and workability in MasterCam.
We searched long and hard for a SW only solution. We found none and would welcome any suggestions/advice/solutions.
Deepak, I hope this helps you understand why we need this, if not I can expand my description in greater detail.
Can your wire department open the sldprt files directly?
What software package do they use? Is it an up to date version that can read SolidWorks files directly?
We save huge amounts of time not generating DXF files for wire by using Esprit.
I would assume MasterCAM can read SolidWorks sldprt files directly as well.
Another option is to save the DXF file from the sldprt file. Select the face and then do a file Save As. This option is not just for sheet metal parts. You can use Draftsight to move the geometry to the appropriate zero location.
We use the latest version of MasterCam. It opens SW files just fine. The problem is I would need to replace my people. The second problem is wire start holes. I can't find a way to make a hole in a cavity in a PRT.
If I need to use DraftSight to move the geometry to the 0-0 position, I might as well use KeyCreator.
I can't help on the better people. We are fortunate to have a bunch of very good toolmakers who are not set in their ways.
Any cad program able to deal with DWG/DXF will work for fine tuning the 2D data.
See attached models for handling wire starts, etc.
Model you wire starts and any back reliefs before your wired cavities. Then create two configurations, milling and final wire.
In the details, the plan view has two views overlaid and aligned. The hole chart is built off the milling operation configuration.
Our machinist's work with the milled configuration for their work. The wire guys can can bring the file into Esprit twice (one of each configuration) to program their wires.
There is no issues with double data, gaps, etc. Engineering gets out of the business of translating data for downstream users.
Thanks for your detailed reply. I got to tell you your method scares the s#$@ out of me.
I now see how you get the WEDM start holes in a cavity.
"In the details, the plan view has two views overlaid and aligned..."
How do you keep them aligned? Can you lock the alignment? I moved one of your views easily and all I can think is the views will get misaligned by a small amount, just enough to scrap the block.
Our WireEDM people are not skilled toolmakers. In fact, this is their very first experience in manufacturing. They are very good at what they do, they just don't have the experience necessary to recognize if something is "off".
I am puzzled how your wire operators have never worked in manufacturing?
If two view overlaid scares you, just do two separate views. One labeled Milling Operation and the other is the final finished part. I overlay the two views to save paper on our smaller die blocks.
Here is another example for you.
We teach in-house what is necessary. Experienced operators teach the new operators. Most of our WEDM work is production (we have 11 machines that run 3 shifts per day). We slowly and carefully train the operators into doing die work. There is an extreme shortage of experienced toolmakers in Connecticut.
My guys would be lost if I only gave them the first print in your PDF. There are no start holes. If I gave them both prints they could manually draw the start holes in MasterCam and hope they don't fat finger the numbers.
Thanks for sharing your experience. I think we will stay with what we are currently doing and continue on looking for a better solution.
In PTC Creo (Pro|E), you can select an origin feature, often a point placed in the model if no corner exists. You can then specifically place the view origin by coordinates. And the DXF output merges all lines and arcs and duplicate removal. This appears to be what SW drawings do also. Obviously I want to remove the external references to create these DXF files. If I could pick the origin of the export file from a drawing DXF export, that would solve the issue.
For laser patterns and such, my provider does nesting and doesn't care. My application is providing PCB data for the layout peeps.
I always export to DXF directly from the part file itself. The content always goes out at 1:1. I can also tell it what orientation/face is normal to and where the origin should be.
I do not mind exporting directly from the model. I am just not sure what to expect when doing this.
How does this method deal with duplication and stops?
I have never had it create duplicates before so not sure about that one. Also, not sure what you mean by stops. In the DXF output options there is a Merge end points but don't know if that is related to your stops. Open one of your parts and give it a go to see if it gets you closer to what you need.
My stops means merging curves that are on top of each other.
I may just hand this over to the VAR to solve. That's why we pay them, right?
I'm not in an experimenting mood.
A quick test shows duplication and merging is working properly (when selected in options).
I've attached the test case. When opened as a import, it has only 7 curves.
This might work.
Retrieving data ...