im wondering how to draw bolt hole circles on a sketch ive attached the sketch
Are you just needing holes for the bolts to go through, or are you needing threaded bolt holes?
If you're just needing simple holes, create a sketch on the surface the holes need to go through. Draw the first circle and dimension it from the center of the part. Then, to save time, you can use the circular pattern tool by selecting the circle to be patterned, the centerpoint as the point to rotate around, and set the number of holes, equal spacing, distance between each, etc. You can also make one hole, and pattern the feature of the hole using the feature circular pattern tool.
They need to be threaded holes thanks for your help im new at this and learning on my own with no help
similar process for threaded holes - just a different size hole. and if you don't want to look up the size for the hole, use the hole wizard for that first hole.
There are a few ways this can be done.
One is Solidworks hole wizard tool. This will create a hole and call it out as threaded, however, as far as I know, it doesn't display the threads. Personally I'm not a fan of that, so I use my second method, which is a bit more convoluted.
For actual full thread display in parts, I make a swept cut of the thread profile. Here are my steps:
1: Find the specifications online for thread dimensions for the thread you wish.
2: Cut a hole with the diameter equal to the minimum inner diameter of the threads.
3: At one edge of the hole, create a sketch along the diameter of the hole at one of the ends of it, for the profile to be cut out for one pitch of the threads.
4. Create a helix on the hole, using the height and pitch settings. Height is how deep you want the threads to be tapped,
5. Use the swept cut tool to sweep the thread sketch along the helix.
I've attached a part I made using this method. Hopefully that can clarify a bit of what I've done...
You really shouldn't cut helical threads into your parts, unless you are using the models to directly create the physical parts (ie. 3D printing). It increases file size and slows rebuild times.
The hole wizard adds a bitmap to the face to indicate that it is threaded. If you just REALLY want to see threads, you can use a simple revolve to cut notches that look like threads.
Good point I should have thought to mention. For simple parts I generally do not worry about the lengthen rebuild time (even with a non-analytical card, I've never had much issue), but if the part is in a complex assembly with multiple fasteners and everything made this way, it can create a load on the machine. If rebuild times do become an issue, then I would go with what the others have suggested. I'm just a stickler on making parts identical to the production part for installation animations and render images, but if that's not an issue, save yourself some pain and suffering and keep it simple using hole wizard
First thing I notice is that none of your sketches are dimensioned.
Why are your sketches not dimensioned?
I delete the dimensions just to get them out of the way. I think my question got derailed alittle bit lol
How are sketch dimensions "in the way".
Deleting sketch dimensions is not considered good modeling practice.
I think Kevin answered your question already but in two different posts. Hope y'all don't mind if I summarize for Mr. Kiefer.
The simplest way to do this, in my opinion, would be to use the Hole Wizard tool. Select the face on which the holes should be drill/tapped. Start a Hole Wizard feature and select the type of hole you want. The hole wizard allows you to specify just about anything about the hole you could ever want to specify: thread type, near/far side countersink, bolt head clearance, etc. Once you've got the type of hole selected, click the "Positions" tab at the top of the Hole Wizard properties manager. This will switch to a sketch on the face that you selected earlier with the "Insert point" tool active. The Hole Wizard simply starts a hole wherever you put a point on that sketch.
To get a circular pattern, the easiest way would be to make the first hole using the hole wizard as I just described. Then make a circle pattern of that Hole Wizard feature. For the circle pattern, you'll need an axis. In the attached example, I used the origin and the front face as references for the axis.
I hope this helps. Be sure to read up on the hole wizard and circle patterns in the help files if you have more questions.
And definitely, leave the dimensions in your sketches. They should only be visible when you go to edit the sketch. It's a good practice to fully constrain all of your sketches using dimensions and relations. You'll know it's constrained when all of the lines turn black. "Black lines goooood, blue lines baaaaad". That's what I always say.
you don't need to add an axis to use the circular pattern feature, you can select any temporary axis (use the view settings to show them for selection) or any circular face, or a linear edge (if there was one in the appropriate place, so not for this model).
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