I'm still new to CAD, new to 3D, new to modeling, new to FreeCAD and first post on the forum. Learned to draft in High School, many years ago. This is my first attempt at modeling with FreeCAD. I'm designing a tailstock turret for my metal lathe. The first part is a rotating head with 6 tool positions. The rotating head will start as 1" thick by 6" round circle. Six holes for tool positions will be bored through the rotating head piece on a 5" circle (one hole every 60 degrees). So far I've gotten this much done (file attached). I need to design one each, set screw hole that will be drilled and tapped from the circumference edge and into each tool holder hole. So far all my attempts to create a sketch to accomplish this have met with failure. Any help would be greatly appreciated!
For me, step-by-step help/advice would probably be appropriate, based on where I am learning FreeCAD.
My system and FreeCAD version information:
OS: Ubuntu 16.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6707 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 5465bc47c95db45e0be85dc0e2872419efadce0f
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
Help request for circumference holes, please
Forum rules
and Helpful information
and Helpful information
IMPORTANT: Please click here and read this first, before asking for help
Also, be nice to others! Read the FreeCAD code of conduct!
Also, be nice to others! Read the FreeCAD code of conduct!
Help request for circumference holes, please
- Attachments
-
- Tailstock Turret Rotating Head.fcstd
- (24.83 KiB) Downloaded 65 times
Re: Help request for circumference holes, please
Welcome to the Forum. There is a steep learning curve but gets easier with practice, practice, practice...and start simple.Inkblotr wrote:I'm still new to CAD, new to 3D, new to modeling, new to FreeCAD and first post on the forum.
You have actually chosen a fairly complex geometry for your first part!Inkblotr wrote: I need to design one each, set screw hole that will be drilled and tapped from the circumference edge and into each tool holder hole.
Sketches require a planar face. Sometimes, due to limitations in V0.16, you have to create a temporary face in order to create a feature. To do so, you have to think ahead a bit which gets easier with experience. Although there may be other ways to accomplish what you want, I suggest the following:
1. Start over.
2. Create your first Pad and include a square located on center with its diagonal equal to the final hole size. You will see later what this is for.
3. Pocket a half hole as shown. This creates a face that you can use later for the radial set screw holes. 4. This is an excellent example to use PartDesign/PolarPattern tool. Copy the half hole feature with this tool using Normal Sketch Axis and six(6) Occurences.
5. Locate a sketch on the planar face of one of the half holes. I used 6 mm radius for the set screw hole in the middle of the pad. Pocket Through All. 6. Copy using the PolarPattern tool but this time "select a reference axis..." which is the edge of the square that corresponds to the center axis as shown below which is highlighted in yellow: 7. Mount a sketch on the Pad face and locate a full circle at the half hole location using an edge on the hole diameter. I used the PartDesign/External Geometry tool for this purpose. This will turn the selected edge magenta. Constrain the hole center and diameter to the external edge.
8. Pocket the hole and copy with the PolarPattern tool as in step 4. 9. Pocket the center hole to remove the temporary square hole.
10. Add the remaining features. Note that you can use the PolarPattern tool.
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
"It is a poor workman who blames his tools..."
Re: Help request for circumference holes, please
ppemawm - THANK YOU for the detailed and step-by-step answer!! I've read your post twice now and I have confidence that I'll be able to follow your instructions. Your technique makes sense based on my previous failed efforts. Without any experience, I couldn't see any path out of the "corner" I designed myself into. I will sit down and concentrate on the steps later this evening, when I have more time.
You are correct, I chose a difficult part to design but didn't think it was, before I started. I don't mind starting over - I respect you for being firm.
Again, my sincerest appreciation for taking the time to write and provide so much information!
You are correct, I chose a difficult part to design but didn't think it was, before I started. I don't mind starting over - I respect you for being firm.
Again, my sincerest appreciation for taking the time to write and provide so much information!
Re: Help request for circumference holes, please
If you do not mind venturing out of the PartDesign workbench there is at least one alternative that you should also investigate as part of the learning process:
1. Starting with your original file as is, create one Part/Cylinder with sufficient length and the diameter of the set screw hole. The cylinder should be longer than the hole that you need (see below). It will be located at the center of the global axis with its axis in the Z direction.
2. Relocate the cylinder using Placement Properties from the Data tab (button with three dots). This is a little confusing at first. You just have to experiment to get the hang of it. First select the cylinder and check the box 'apply incremental changes'. Rotate the cylinder about the Y axis 90 deg. Translate in the X direction to the approximate location shown. Translate in the Z direction to center it. Select Apply. 3. Use Draft/Array to create a polar array of six cylinders about the Z axis. All of the array properties are defined in the data tab in the Combo view. 4. Subtract (Cut) the cylinder array from the last feature of your file (Index Pin Holes) using the Part/Make a cut of two shapes tool. Select the last feature and CTRL select the array from the Model tree then apply the Boolean cut tool.
With this approach you can salvage what you have already completed. There is almost always several ways to accomplish the same result in CAD software.
1. Starting with your original file as is, create one Part/Cylinder with sufficient length and the diameter of the set screw hole. The cylinder should be longer than the hole that you need (see below). It will be located at the center of the global axis with its axis in the Z direction.
2. Relocate the cylinder using Placement Properties from the Data tab (button with three dots). This is a little confusing at first. You just have to experiment to get the hang of it. First select the cylinder and check the box 'apply incremental changes'. Rotate the cylinder about the Y axis 90 deg. Translate in the X direction to the approximate location shown. Translate in the Z direction to center it. Select Apply. 3. Use Draft/Array to create a polar array of six cylinders about the Z axis. All of the array properties are defined in the data tab in the Combo view. 4. Subtract (Cut) the cylinder array from the last feature of your file (Index Pin Holes) using the Part/Make a cut of two shapes tool. Select the last feature and CTRL select the array from the Model tree then apply the Boolean cut tool.
With this approach you can salvage what you have already completed. There is almost always several ways to accomplish the same result in CAD software.
"It is a poor workman who blames his tools..."
Re: Help request for circumference holes, please
Wow, you make it look so easy! Your second reply is close to what I had tried miserably to do for a couple of evenings before finally giving up and posting my question. I'm a little confused, please.
You mention if I didn't mind venturing outside the Part Design workbench... (I don't mind and am excited to go here) but in step #1 you don't mention which workbench I should use to create the first set screw cylinder? I understand it will be centered on the global Z axis.
In step #2 the relocation of the cylinder (created in step #1 above), was that effort more complicated because the first PAD (creating the circular disk) I didn't specify the pad to be symmetrical to the sketch plane? I realized I should have probably checked the 'symmetry' box when I executed the pad much later. I didn't know if I could go back and change that, but I'm thinking now it is possible and I should do that?
The remaining steps in your second post I understand and I will follow.
Thank you so very much for the all your time and effort to help me!
You mention if I didn't mind venturing outside the Part Design workbench... (I don't mind and am excited to go here) but in step #1 you don't mention which workbench I should use to create the first set screw cylinder? I understand it will be centered on the global Z axis.
In step #2 the relocation of the cylinder (created in step #1 above), was that effort more complicated because the first PAD (creating the circular disk) I didn't specify the pad to be symmetrical to the sketch plane? I realized I should have probably checked the 'symmetry' box when I executed the pad much later. I didn't know if I could go back and change that, but I'm thinking now it is possible and I should do that?
The remaining steps in your second post I understand and I will follow.
Thank you so very much for the all your time and effort to help me!
Re: Help request for circumference holes, please
Hi Inkblotr, and welcome!
http://freecadweb.org/wiki/index.php?title=Part_Module
That's what he meant in the text I colored green:
@Inkblotr, click the Create Cylinder tool in FreeCAD, then use the Data tab (lower left corner of the FreeCAD window by default) to change the Properties of the newly created Cylinder.
@ppemawm, please correct anything I've misinterpreted or goofed up.
Part WB (not Part Design):Inkblotr wrote:You mention if I didn't mind venturing outside the Part Design workbench... (I don't mind and am excited to go here) but in step #1 you don't mention which workbench I should use to create the first set screw cylinder?
http://freecadweb.org/wiki/index.php?title=Part_Module
That's what he meant in the text I colored green:
(@ppemawm, I like to type it like "Part WB > Create Cylinder tool" - seems to make it easier for newcomers to understand)ppemawm wrote:1. Starting with your original file as is, create one Part/Cylinder
@Inkblotr, click the Create Cylinder tool in FreeCAD, then use the Data tab (lower left corner of the FreeCAD window by default) to change the Properties of the newly created Cylinder.
In this method the default Part WB > Cylinder is created without using a Sketch.Inkblotr wrote:In step #2 the relocation of the cylinder (created in step #1 above), was that effort more complicated because the first PAD (creating the circular disk) I didn't specify the pad to be symmetrical to the sketch plane?
- Part Design WB is always for creating solids, and usually a single solid. Separate solids can be created but in 0.16 they are unaware of one another in the Part Design WB. This changes in FreeCAD 0.17.
- Part WB can create other things too (not only solids) and recognizes them as separate items if you keep them separate.
Yes it's possible using the Property in the Data tab again. (The Pad needs to be selected in the history tree first).Inkblotr wrote: I realized I should have probably checked the 'symmetry' box when I executed the pad much later. I didn't know if I could go back and change that, but I'm thinking now it is possible
@ppemawm, please correct anything I've misinterpreted or goofed up.
Re: Help request for circumference holes, please
I missed some things in that last post:
It usually is easy, once you learn how.Inkblotr wrote:Wow, you make it look so easy!
Don't wait so long to ask for help here, replies usually happen quickly.Inkblotr wrote:I had tried miserably to do for a couple of evenings before finally giving up and posting my question.
At first it may seem overwhelming when and why to use a particular WorkBench, or even a tool from a particular WorkBench without becoming proficient in any one WB. Eventually you will have to change WB's when working on a model though.Inkblotr wrote:You mention if I didn't mind venturing outside the Part Design workbench.
Re: Help request for circumference holes, please
Thanks for the help and clarification.bejant wrote:@ppemawm, please correct anything I've misinterpreted or goofed up.
"It is a poor workman who blames his tools..."