AutoCAD user learning SolidWorks

[V8Goose]

Hi and thanks for looking...

 

As a very experienced AutoCAD user trying to teach myself SW, I gotta say the frustration level is quite high.

 

I'm not complaining, SW is the correct product for a small project I am doing, but man... it seems the concept behind how to design in SW still escapes me (and I'm running out of hair to pull out! )

 

Anyways... I am wondering if this forum is a good place to get help. I'm not looking for charity, I DO research, try, read, do tutorials etc but there are some things that I just do not understand.

 

For example:

I have created a small part (see part_1). The next part has similar cylinders and must join this part in the same place.

 

So I insert this part into the next drawing and try and use it to create the adjoining piece.

 

First issue is that I don't know how to place the inserted piece so that the cylinders are on the top plane, nor can I move it to be so.

 

I also cannot create a new plane by selecting the cylinder faces because I need more definition points.

 

Anything I sketch (centerline, circles etc) become a child of the inserted part and therefore when I delete the insert, my new parts go with it.

 

It seems I cannot dissassociate the children from the parent and move them up the stack.

 

I'm at a loss... how do I use my existing part as a template to build the next one?

 

Many thanks!

 

Goose

[shift1313]

Welcome aboard goose, this is the right place:)

 

Im having a little trouble following what the end part is going to be but ill try to help you out.

 

What version of SW are you using currently?

 

Some basics. You have 2 major file types to work with, Parts and Assemblies. When you create a part, it can be a single solid body, or multiple solid bodies(or surfaces but we wont talk about that for this situation). The modeling approach is very different from Acad as you said. And one of these difference which you have found in your case is History. SW models are based on parameters and the features in the model tree. Think of it as sort of a timeline. If you delete a part, you are deleting everything in the tree associated with it, and that means any of those features you used to create other things. There is a way around this. At the top of the feature tree there will be a folder called "Solid Bodies". If you expand this and right click on the body you wish to remove you will see a function called "delete body". This isnt the same as the delete key, but rather its a feature that gets added to the tree. This means everything dealing with that solid before the "delete body" will still be available and usable.

 

If you can maybe break down the design of what you are trying to do I can walk you through it step by step. Im just a little unclear on where the two parts are and what features you need to use from one for the other.

[V8Goose]

Hi Matt...

 

Thanks for the quick reply.

 

My apologies for lack of detail. Lets see... I'm using v2009.

 

I understand the difference between parts and assemblies, right now I am trying to create several parts for one final assembly.

 

The part_1 picture above is a plastic frame for a gearbox and electric motor assembly. Lets call this the bottom. The top of this frame is almost a vertical mirror of this part and the two vertical cylinders are screwed together with screws down inside the top cylinders.

 

This is where I wanted to insert part_1 into the next drawing (i know i shouldnt use the word 'drawing' as it means something else in SW) called say Part_2, and draw off it so that when I assemble the parts (in an assembly) the sizes and locations of the mating cylinders are correct.

 

Aligning the inserted part with the top frame for example, has been thus far impossible, whether I try to do it as the part is inserted, or moving it after the fact. I'm sure its simple, but I haven't figured it out yet.

 

Once the top part is drawn, I intended to delete part_1 (thanks a lot for the explanation about the tree), save part_2 and move on to the next part until they are all created and ready for assembly.

 

Thats a long winded way of explaning it, but I hope it makes sense.

 

Thanks for your help.

 

Goose

 

PS: By some act of God, it seems that I can now add a frame and the two cylinders I was talking about (see part_1_1) however deleting the solid body in the tree still removes the entire assembly.

 

Is that because of how I created the cylinders?

 

Cheers

[V8Goose]

So through lots of trial and error/reading... I managed to complete the top part of the frame including an interesting fight with an 'open loop'.

You would think that drawing two circles on a plane and then a line from the top tangent to the other top tangent, repeating that for the bottom, and then using the trim tool would create a closed path, but not for me!

 

Anyways... to better explain why I can't seem to delete the solid bodies of the inserted part, please check out Part_2 showing the tree in which Frame_2 is the inserted part.

 

And then Part_2_2 which is the highlighted selection when I choose delete solid body under Frame_2 in the tree.

 

Eek!

 

I don't understand why it is selecting (Frame_2) & (Extrude5) in the selection set.

 

Any idea's.

 

Promise to leave you all alone after this piece... that's about all the stress I can take for tonight

 

Cheers

 

Goose

[bhamze]

Welcome Goose,

 

Its been awhile since I used AC and I can still remember the headaches transitioning to SW. However, once you understand SW and its tools you"ll find it hard going back to AC. I would recommend you do all the SW tutorials located in the help menu, it definitely helped me. I know the learning curve is frustrating, but having AC experience is a plus, you have an understanding of how to create geometry and the rules for creating them. If you ever get stuck, you've found the right place. The people here really go out of their way to solve problems. You've already meet Matt, he offers great advice and is always willing to help.

 

From what I can see in the picture. You created a part and inserted it into a new part then added the cylinder features. Is this correct? I also noticed only one solid body. If you intend to have multiple bodies in a single part you must uncheck the merge results feature. Check the extrude feature that you last created, the merge result feature is checked. If it wasn't, the solid bodies folder would have 4 bodies.

 

I think a better approach would be to create an assembly with the frame part. In an assembly you can create a new part that references features on the frame part. For example........you can click one of the cylinder faces on the frame as the sketch plane. Then create a circle that is concentric from that selection. Extrude the sketch then exit. You now will have two separate part files that can be edited, hidden, or deleted (depending on its relation).

 

Can you attach file? I can take a look for you.

[shift1313]

Goose, I think bill hit the nail on the head. In an assembly you can create new parts and project geometry into your new parts. There are benefits to this and draw backs as well. Typically I try to draw parts separately without using external links, because they get messy and cause headaches. For this part you should know the distance between the "pins" so creating a new part should be straight forward. There is also the ability to use Blocks just like in acad. You could create a block from one part, save it, then insert that block into another parts sketch with no link between the two.

 

Ill try to draw up a quick example for you here in a little bit(hopefully) on how to convert things. I have 2009 so everything should look the same for you.

[shift1313]

Hey goose, i threw together some pictures but the last time i typed this my firefox browser crashed. Im just going to upload the pics and if they need any clarification we can discuss it in another post.

[shift1313]

Alright, ill try to explain the overall proceedure since the pictures went up last night just fine. After I had the main part drawn, i selected the end face of one of the extrusions. I didnt need to do this, but since these parts won't actually be fitting together here that seemed like a good place to start. In my sketch I use the Convert Entities button to bring in the circular edges. Note: in the real world these would not be the exact size and you could just click the edge and use Offset Entities without having to convert them, but for this example I neglected the perfect fit. I then offset these converted edges to make two closed cylinder profiles that I could extrude.

 

During the Extrude dialog you will want to uncheck the Merge Results box. I explained in the picture, but this is essentially UNION from ACAD. It will merge any solid bodies that contact each other. Now an interesting note, if you uncheck this box and extrude these cylinders, they will be two parts, leaving you with three solid bodies.

 

Next I created a sketch at the end of these for their base plate. Here you want to check the merge results box, but in the Feature Scope box you need to make sure that "All Bodies" isnt selected and that "Auto-Select" isnt selected. Auto-select will join any solids that are touching so you will again end up with one solid. You will want to select the two tubes we just extruded as your feature scope and it will join these two with the plate. Now you should have two solid bodies.

 

In the solid bodies folder, right click on one of the parts and select Insert into new part... This will export this part into a new file. Do this for both files, then create a new assembly and insert both files into the assembly. You will not be able to modify these new parts. You will have to come back to this multi-body solid and make your edits. As long as you dont break the references between the files they will update accordingly.

 

Let me know if you have any questions. This is one of many ways to go about this but probably the easiest method with the lowest risk of causing reference failures and broken links.

[V8Goose]

Thank you one and all for this wealth of information.

 

It appears a combination of the Merge setting and my limited knowledge was the reason for my dilemma.

 

I will no doubt have more wierd questions for you as I progress, starting again tonight.

 

Cheers!

 

Goose

[V8Goose]

Here is another couple of things that are driving me crazy...

 

For example 1: I just drew a line and set it to a specific length. I then drew a circle on each end. Now when i delete the line (from the tree) I get error messages talking about dangling sketch entities. I can't delete construction items?

 

2. How do I query items? I want to know how far it is between points or the diameter of a circle or cylinder. Is dimensioning the only way?

 

Thanks as always...

 

Goose

[shift1313]

Well the approach to defining a sketch is different from how you do it in ACAD. you need to dimension your sketches. If you need a circle a certain distance form something, add a dimension to it. This is not in the properties window off to the left, but actually adding a dimension. Also make use of relations. You can add a horizontal relation between the center point of the circle and the origin. then you can add a dimension and this will locate your circle.

 

2. Under the tools menu there is a Measure function. But you still need to define your sketches. The bottom of the window should have something that says Fully Defined or Under Defined. Also your sketch lines and items will be blue when they are not defined, and turn black when they are.

 

Here are some documents I wrote.

 

http://filebox.vt.edu/users/maperez/SolidWorks%20Tutorials/SW%20Tutorial%20(2).zip

 

They are all lumped together but #4 is what you want to look at. I talked about defining sketches.

[V8Goose]

Would one of you noble sages please, for the love of god, tell me what is wrong with the attached file and how to fix it?

 

The error message says the reference plane is missing. I probably deleted it. Now that I am starting to understand how all the geometry is 'linked' I wont be deleting stuff.

 

So accepting there is an error, I used Edit>Sketch Plane as instructed but am stumped how to satisfy the command into inserting a new plane.

 

I'm all for teaching a man to fish, but my family is going to starve!

 

Many thanks

 

Goose

 

File attachment won't work for me, the file is on my site here... (9 post minimum) www dot goosesworld dot com / dump / Spring_1.SLDPRT

 

PS: Excellent! Thanks Matt...

 

PPS: That's all I can take for tonight...*sleep*

[shift1313]

Hey goose, there is nothing attached, but the location of everything in the feature tree is important. If you create a new plane after the feature that has the problem in the tree, the feature wont know the plane is there. It builds on itself in a way. You can drag the features up the tree and you can also right click on them and see parent/child info.

[bhamze]

Would one of you noble sages please, for the love of god, tell me what is wrong with the attached file and how to fix it?

 

The error message says the reference plane is missing. I probably deleted it. Now that I am starting to understand how all the geometry is 'linked' I wont be deleting stuff.

 

So accepting there is an error, I used Edit>Sketch Plane as instructed but am stumped how to satisfy the command into inserting a new plane.

 

I'm all for teaching a man to fish, but my family is going to starve!

 

Many thanks

 

Goose

 

File attachment won't work for me, the file is on my site here... (9 post minimum) www dot goosesworld dot com / dump / Spring_1.SLDPRT

 

PS: Excellent! Thanks Matt...

 

PPS: That's all I can take for tonight...*sleep*

 

 

Right click Sweep3 then select delete. When Confirm Delete dialog box appears, make sure also delete absorbed features is unchecked. Select yes. If prompted, close Whats Wrong dialog box. Place mouse pointer on blue line under sketch4 in feature tree. The mouse pointer will turn into a hand, left mouse click (hold down) and drag blue line under helix/spiral2. Add a new plane, click reference geometry then add plane. Under first reference click Helix/Spiral. Under second reference click bottom point of Helix/Spiral

(make sure coincident is selected). Click green check mark. Place mouse pointer on blue line again, when hand appears left mouse click (hold down) and drag blue line under sketch4. Right click sketch4 and choose edit sketch plane. You may need to expand Spring part (click + symbol located just right of feature tree) select plane1 then green check mark. Your sketch is now repaired. Redo your Swept Boss/Base feature and your done.

[bhamze]

Hey goose, there is nothing attached, but the location of everything in the feature tree is important. If you create a new plane after the feature that has the problem in the tree, the feature wont know the plane is there. It builds on itself in a way. You can drag the features up the tree and you can also right click on them and see parent/child info.

 

Hey Matt. How r things? Here is the link for the Goose .

 

http://www.goosesworld.com/dump/Spring_1.SLDPRT

[V8Goose]

Thanks a lot Bhamze...

 

I was able to follow your instructions until inserting the new plane.

 

I don't understand the part where you say "...Under the first reference..."

 

This is what I see when attempting to insert a new plane...

 

 

There seems to be only one reference (the blue box, right?) so there is something I am doing wrong.

 

Thanks again to all of you for your help, much appreciated.

 

Goose

 

PS: I have a lot of difficulty creating planes, for example I am trying to insert one in the part above but I don't seem to have enough reference points (face, point, line, edge) to satisfy the creation process and I have tried to define it though all of the available methods (Through lines/points, Parallel at point, normal to curve or on surface).

I have an end point and the helix which is not a line, edge or face.

[shift1313]

If you right click on the sketch in question(its name in the feature tree) there is an icon next to edit sketch if your quick menus are on shown in the attached image. This will let you pick a new sketch plane to replace the bad reference or delete plane/planar face.

[bhamze]

Thanks a lot Bhamze...

 

I was able to follow your instructions until inserting the new plane.

 

I don't understand the part where you say "...Under the first reference..."

 

This is what I see when attempting to insert a new plane...

 

 

There seems to be only one reference (the blue box, right?) so there is something I am doing wrong.

 

Thanks again to all of you for your help, much appreciated.

 

Goose

 

PS: I have a lot of difficulty creating planes, for example I am trying to insert one in the part above but I don't seem to have enough reference points (face, point, line, edge) to satisfy the creation process and I have tried to define it though all of the available methods (Through lines/points, Parallel at point, normal to curve or on surface).

I have an end point and the helix which is not a line, edge or face.

 

 

I see the problem. I'm using SW2010, your using an older version. In 2010 there are more options for creating planes.

 

When you create your new plane do not select any options under the selection box. Just select your geometry, if selected geometry is suitable the software should create a plane automatically. In the selections box, first select the helix/spiral then select the bottom point of the helix/spiral. You will see your two selections in dialog box. This will create the new plane. Follow the other procedures to complete the sketch.

[V8Goose]

Hi again...

 

The older version combined with my current skill level equals some hair-tearing times...

 

Here is what happens when I try to create a plane by selecting the helix followed by the end point...

 

dubdubdub dot goosesworld dot com / sw / plane_1.swf dot html

 

Is there a way to rotate a plane by selecting say the origin and a point?

 

Please let me know if this is an acceptable method of showing you whats going on.

 

Many thanks

 

Goose

[shift1313]

goose, i couldnt get your site based on that. im sure i just typed something wrong.

 

To create a plane at an angle you need a plane as a reverence and either an edge or an axis(which could be 2 points). Out of curiosity are you trying to rotate the plane at the end of your helix? What are you trying to draw here with the helix? there are other ways if you are trying to draw a spring or something similar.