Part Design + Text String Generates 1,000 meshes???

[cad dog]

normandc, thanks for your post "IMPORTANT: Please read first before asking for help", it was very informative. Attached is the table's .FCStd file you requested. Also, it looks like I have both the 32-bit and 64-bit versions of FreeCAD exe's on my computer. Here is the "About FreeCAD" info of both.

OS: Windows
Word size: 64-bit
Version: 0.14.3700 (Git)
Branch: releases/FreeCAD-0-14
Hash: 32f5aae0a64333ec8d5d160dbc46e690510c8fe1
Python version: 2.7.6
Qt version: 4.8.5
Coin version: 4.0.0a
SoQt version: 1.6.0a
OCC version: 6.6.0


OS: Windows
Word size: 32-bit
Version: 0.14.3700 (Git)
Branch: releases/FreeCAD-0-14
Hash: 32f5aae0a64333ec8d5d160dbc46e690510c8fe1
Python version: 2.6.2
Qt version: 4.5.2
Coin version: 3.1.0
SoQt version: 1.4.1
OCC version: 6.5.1

My operating system is Windows 8 64-bit and when I use the 64-bit version of FreeCAD mentioned above, then selecting Pad004 highlights the table top and all four legs together in the gui and selecting any of the other Pads 1 - 3 does not highlight anything in the gui. Shouldn't I be able to highlight each of the pads separately in the gui?

When I use the 32-bit version of FreeCAD that's when I get the Pad highlight issues mentioned in my last post, so the 32-bit and 64-bit versions of FreeCAD are not playing nice with each other as they each give different results. Even so it looks like neither version is giving me the Pad highlight functionality I expected in the gui. Please advise.

[bejant]

The file makes it easy, toggle visibility of Pad001 to Off, then select Pad004.

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Edit:

20141122c.png (49.08 KiB) Viewed 1606 times

[sgrogan]

The help on FreeCAD helps alot.

Windows 32 was compiled with much older libraries so it is not as advanced as the 64 bit version.

You should also state which workbench(s) you are using. In this case, from your file Part Design.

Part Design Workbench is designed to build up a Single Solid.

In your case you have 3 solids.

Go to tools > Dependency Graph

If you get an error because it is not installed, google graphviz. There is a window$ installer. Downlowd, install, etc from the graphviz site. Then back in FreeCAD Tools>Dependecy graph

You will see you have 3 solids.

Pad004 is "built up from your original Table sketch.

I think you want 2 solids. Onne of the table with the text "subtracted" form the table. I don't know the functionallity of shape string so I will have to defer to the experts.

You need to "subtract" one of your shape string extrudes, Boolean difference from the part work bench.

I think then you will have two solids, ready for your dual extruder project.

BTW: How many extruders do you have(invision)

[NormandC]

Thanks for finally posting your FreeCAD info.

Also, it looks like I have both the 32-bit and 64-bit versions of FreeCAD exe's on my computer.

You should need only one version, preferably the one with the same 64-bit architecture as your operating system. As each version's pasted info shows, the 64-bit one has more recent software libraries (higher version numbers). The most important here is OCC (Open CasCade), which is the geometric modeling kernel on which FreeCAD is based on. 2D/3D geometry creation relies on it. OCC 6.5.1 is now quite outdated.

Shouldn't I be able to highlight each of the pads separately in the gui?

There's something important to know about how the Part Design workbench works. Its tools do not create new objects, but operations (or steps) in the creation of a part. We call those operations "features".

What makes it a new part or not is actually the manner in which you create a new sketch. When using the plane selection dialog window (with the choices of standard XY, XZ and YZ planes), creating a sketch is the process of starting a new part. The first Part Design feature that you build from this sketch (Pad or Revolution) is called a base feature, in other words the first feature that creates a solid.

Afterwards, when you map a sketch to the face of a feature, you're linking the sketch to it, which fuses any feature you build from it with the feature the sketch was mapped to. The new feature becomes the latest representation of your part, and the prior one is automatically hidden. When mapping a sketch to a feature, you get access to material removal features such as Pocket and Groove, which make use of boolean operations union and cut unnecessary.

So looking at your file, all the pads in your file are the different steps in the creation of a single part (the table). You can see this when you toggle visibility from Pad to Pad004.

As bejant said, to export the table, only Pad004 should be selected.

I hope this explanation was clear. I suggest you read a reply I wrote a long time ago that goes through modeling of a simple part using Part Design features. It also might give you a few ideas. For example, you didn't need to create four different pads for the table legs. You could have applied a PartDesign MultiTransform feature on Pad001 containing two mirrored features, one on the vertical axis and the other on the horizontal axis.

A couple tips about constraining sketches: prefer the use of geometric constraints over dimensional constraints.

• In the "Table" sketch, the rectangle could have been centered on the origin with a single Constraint Symmetric on two diagonally opposed points and the origin point
• In Sketch001, an equal length constraint between one horizontal and one vertical line would avoid use of two dimensional constraints.

[NormandC]

sgrogan replied while I was writting my own reply, sorry for the repeat, and I forgot about an important one:

I think you want 2 solids. Onne of the table with the text "subtracted" form the table. I don't know the functionallity of shape string so I will have to defer to the experts.

You need to "subtract" one of your shape string extrudes, Boolean difference from the part work bench.

Yes, otherwise your table will never export with engraved text.

But you actually have three "solids" since you have two Extrude ShapeString objects. What's needed here is

1. Select both Extrude and Extrude001 and click on the Part Union tool, this will create a "Fuse" object
2. Select first Pad004 then "Fuse", and click on the Part Cut tool; this will cut out the extruded text from the table top and create a new "Cut" object.
3. Export "Cut" to STL
4. Reveal the nested shapes under Cut, select Fusion to export the two sets of text strings as a single STL file.

BTW I just noticed that the digits are only 11mm high. I hope your 3D printer has extremely high resolution. I know mine would struggle with so tiny details.

[cad dog]

'sgrogan wrote:
"BTW: How many extruders do you have(invision)"

Thanks for your help. I'm running a dual extruder now because that's the max # Lulzbot supports for their Taz 4 printer. They also have a dual extruder specifically designed for ninjaflex so I could run something like ninjaflex ext0 / plastic ext1 or vise versa. I'm looking at buying one along w/ a second Taz 4 to make composite rubber / plastic parts.

I looked at the Cubex Trio, but did not see good reviews about their printers in various forums / on Amazon and I was concerned about being locked into their proprietary cartridges. Wasn't sure I'd be able to jail break their printers to use any vendor's plastic.

I'd be interested to hear if you know of any good dual, trio, etc printers out there that are supported by the mfg...I have a lot of parts to design / print and don't have much time to customize my printers; hence the reason I prefer mfg support on multi-extruders. I had a Rostock Max and spent more time modifying the printer to do what I want than I did printing the parts I need...prefer not to go down that road again.

[cad dog]

normandc, thank you for the very informative follow up.

For example, you didn't need to create four different pads for the table legs. You could have applied a PartDesign MultiTransform feature on Pad001 containing two mirrored features, one on the vertical axis and the other on the horizontal axis.

You happened to mention something I need for the table's grid lines. I created a rectangular grid line with width / depth about 0.12 inches. It's called Pad006 in the attached FCStd. I highlighted Pad006 and used PartDesign MultiTransform feature to create LinearPattern so I'd have 7 grid line lining up with some of the numbers. Please let me know why I can only see Pad006 in the gui and not all the other grid lines I created with MultiTransform (see pic below).

[NormandC]

Pad006 is not linked to the table part, for which the last feature is Pad004. The PartDesign transformation tools can only work if they have a support (base solid) large enough so the repeats of the patterned feature do not lie in empty space. Which is the case with your LinearPattern feature.

Think of a hole (pocket feature) on a plate that you would pattern on it. There cannot be holes if the occurrences are out of the plate.

What's odd is that it should advise you of the error. But you can still see it in the 3D preview. The fact that it shows the occurrences in red is a tale sign it's not working.

LinearPattern_missing_support_01.png (7.98 KiB) Viewed 1542 times

If you want to make repetitions of disjointed bodies, the Draft Array tool is more suited.

[NormandC]

I just had a look at the sketches in your latest file. Remember what I wrote about dimensional constraints.

A couple tips about constraining sketches: prefer the use of geometric constraints over dimensional constraints.

[cad dog]

Pad006 is not linked to the table part, for which the last feature is Pad004.

I originally tried to make the gridlines on the table sketch itself, but when I added the rectangle to the table's sketch it cut a hole in the table and one of the legs disappeared (see pic). Do you know why these things happened instead of just letting me add the additional sketching of the rectangle to the table sketch? The FCStd file is attached.