With the final drawing for the shaker table completed in the previous installment of this Inventor Tutorial, its finally time to start extruding some features. To prepare for extruding, turn on the visibility of all sketches except the first one, the Top Sketch.
You should now have a screen that looks something like this…
The first extrusion will be the front leg profile –the rectangle less the taper. Select the Extrude tool from the Create Panel, and click inside of the leg shape. Note that the green lines (depending on color scheme) represent closed loops –all of which can be chosen for this particular operation. After selecting the front leg profile, click the little arrow on the right hand side of the text box and choose “List Parameters”. Choose Leg_Width from the list…
You now have the beginning of the leg –but its only tapered on the one side. Shaker legs have both inner faces tapered, which is why we have the second leg sketch. We will now create the second taper by grabbing the Extrude tool, and changing the default “Join” operation to a “Cut” operation, and clicking on the taper part of the LEFT (look at the View Cube) facing sketch. To the left of the text box on the Heads-Up display, click the little down arrow and choose “Through all”, then click the green check mark to finish the operation. You now have one tapered leg.
With the leg complete, we can finally get to the mortise and tenon joint that started this whole tutorial.
The Cut extrusions that make up the mortises that we are about to create are a tad different than the average bread & butter cuts in that they have their sketch on one plane and start & stop on two others. To begin with, expand the Tenon Bottom Plane in the browser to reveal the Tenon Top Plane beneath. Now select the Extrude tool to begin the operation. Pick one of the mortise/tenon profiles as seen in the image below, then use the little arrow to the left of the text box in the heads-up display to change the Extents of the operation to “Between two faces/planes”…
…then select the Tenon Top Plane and the Tenon Bottom Plane to specify the extents of the operation. Now repeat this operation for the other mortise, and name them Mortise A (front) and Mortise B (Left).
Note: The order in which you choose the planes will depend on the direction of the extrusion, which unfortunately must be selected before you get to the ‘Between’ Extents screen as the directional controls, for some strange reason, are not available there (it is present on the ‘heads-up’ version of the tool, but is grayed out).
I may need to do a How-To on this as it can be a bit confusing, but until then, if you are getting an error, you need to change the order of your plane selection or start over and flip the direction to the opposite of what you started with…
Now for the tenons. To begin with, expand the Solid Bodies folder in the Feature Browser (up at the top), name the solid body there Leg A, then right click it and make it invisible. Now start an Extrude operation. We will repeat what we did for the mortise operation with two exceptions, we will leave the operation as the default “Join” operation, and we will select New Solid from the Operation drop down list…
You should wind up with a tenon like the one below…
Because the mortise and tenon were created using the exact same geometry and parameters, they will always remain a perfect fit no matter how much resizing goes on later.
Now for the apron that is connected to this tenon. This is a simple Join extrusion. Start the Extrude command, and select the front apron profile as shown below. Select Apron_Width from the parameters list as the extents, and make sure the dashed magenta line encompasses the tenon (it will also highlight the tenon solid in the Feature Browser’s Solid Bodies folder)…
These two features are now combined into a second solid. Rename the solid Apron A in the Solid Bodies folder. Now start another Extrude operation and select the other tenon profile. By default, the program will assume that this new extrusion is another feature on the second solid (which is correct). Choose New Solid from the Operation drop down menu to set the program straight…
Then name the new solid Apron B. You should have something that looks like the image below at this point…
Now add the apron’s body to the tenon as was done earlier on the other apron…
Now for the corner bracket. Make sure it becomes a new solid body, use the Apron_Width parameter for the Extents, and name it Corner Bracket…
The last extrusion will create the Top solid. For this extrusion, shut off the visibility of all sketches except the first one, the Top Sketch, then extrude that sketch in the Z- direction using the Top_Thickness parameter to define the extents…
If you did not make the Top a new solid, you can go back and double click on the extrusion and select “New Solid” in the Operation drop down to do so now.
That concludes today’s session. Stop back for the next installment of this fine Inventor tutorial where pattern what we have into a full table. See you then…
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Hi Mark… I'm having some trouble with a part of this tutorial…
When creating the solid for "Apron A" if I select Join from the drop-down then no solid appears. If I select "New Solid" then it does. However in the steps it says "(and make sure the dashed magenta line encompasses the tenon (it will also highlight the tenon solid in the Feature Browser’s Solid Bodies folder))". That's not happening for me. Any idea what might be happening? I do have both mortises and both tenons created and they seem okay.
What's unclear to me – how does Inventor know not to boolean join the apron to the leg as opposed to the tenon?
Thanks for any help.
Mark
Hi Mark,
Sorry for the delay, I was out of town and incommunicado over the weekend.
I’m not quite sure what is going on your side, but it sounds like you are combining two separate steps. The creation of the Apron A solid is when the Tenon A Feature is created –this is the only time you would use the “Create New Solid” command on the apron. The body of the apron is just another feature on that same solid, and when you mirror, you are mirroring both features, but again, it remains the same solid that was created back at the Tenon A feature (in a given part you can have hundreds of solid bodies –each containing numerous features of all sorts. The same model could be made as just one giant part if you never use the “Create New Solid” tool).
The Apron A part begins at: “Now for the tenons. To begin with, expand the Solid Bodies folder” ——-which may be where the confusion creeps in. On a side note, and to add more confusion, there is also a tool that you can use to choose what solid you wish a new feature to become a member of. It is just below the Profile tool on the Extrude menu (or on a drop-down in the mini heads-up version) If you are clicking on that, weirdness may happen depending on the exact circumstances.
If you are still having trouble, just let me know and maybe I’ll create a quickie video that walks thru solid body creation.
Update, the second part of your question about how Inventor knows what to join to what –I think it tries to join to a visible feature before an invisible one, the last feature before a feature created earlier, and a few other priorities….but I didn’t write the code so I can’t say for sure. What I can say, is that the “Solids” selector tool briefly described above is what you use to tell the program what solid a feature is to become a member of. This is covered in one of the tutorials in the menu to the left, but may make a good, brief little tutorial all on its own.
Thanks for the feedback, Mark. With your comments I've been able to get Inventor to join or create new solids as I need now.
This sentence may be the issue (or not – I could be wrong!): "We will repeat what we did for the mortise operation with two exceptions, we will leave the operation as the default “Join” operation, and we will select New Solid from the Operation drop down list…". It feels like if you make a new solid you are no longer joining.
In any case – great tutorial – I learned a lot.
Thanks,
Mark
Hi Mark, I see what you mean about the “Join” operation, I generally leave the settings be (Join by default), select my closed loop, then select the “New solid” option. It can be done the other way around –not sure if there is a benefit either way. If any other readers have any input, it would be interesting to hear.
While I’m here, I may as well let people know that I’ve been dealing with a Windows 7 Update that hosed my primary system all day today since minutes after posting installment #7 . It was like a flashback to Windows 98…
I promise I’ll get out a post on either iLogic or adding a semi realistic color and material tomorrow (12-22-11).
Hi Mark and Mark. I'm hoping that I can shed some light on Marks question about the apron not showing up during the extrude command. I have noticed that as you are building your model, there seems to be a very specific need for selections in a specific order. I have had this situation happen before and it seems to be from jumping a step, or selecting "new solid" by accident and re-selecting "join". A few odd combinations later and sure enough, the program that automatically selected the tenon for joining, now is un-selected. When this happens and you select "join" for your apron, nothing shows up until you re-select the tenon.
Another example is that if you made Tenon A as a solid body, then skipped ahead and made Tenon B as a solid body, then jumped back and started working on your apron, the join command is default selected, but when you select the profile for the apron, nothing shows up. This is because the software has not selected either of the tenons.
I was a bit confused at first with this comment:
"We will repeat what we did for the mortise operation with two exceptions, we will leave the operation as the default “Join” operation, and we will select New Solid from the Operation drop down list…"
While I knew what you were getting at, I thought for a second that I may be going batty since one can only select either "solid body" or "join", not both. I was thinking that I was missing a step somewhere.
I was wondering if you would expand on this comment
"…then select the Tenon Top Plane and the Tenon Bottom Plane (must be in that order)…"
I was curious as to why it must be in that order. I tried it both ways and it seems to work, but I'm guessing it may have something to do with how it is stacked in the browser or how it will be handled in a mirror command.
Thanks again Mark, great stuff.
Hi Kent,
With multi-solid bodies, the order of execution is VERY important. When Autodesk first introduced them, I was getting the order wrong for quite some time (I can be a tad dense). There are a couple of pages I created on solid bodies that may shed a bit of light:
Mirror Multi-Solid Bodies and Cutting Multi-Solid Bodies
Both can be found in the How-To section in the menu to the left.
You are correct about the “join” statement, instead of saying leave it at the default, I should have said just skip right over the normal operations to the New Solid operation which is by itself just below them. I’ll do some editing … thanks for the head’s up!
The last one is a tad tricky. If one were following along with no diversions, their extrude direction should have been the same as mine, which would necessitate that particular order of selection. The direction must be set BEFORE selecting ‘Between’ as the Extents. Once you have Between selected, if your direction is up, you will get the Error:
The feature as specified did not change the number of faces (and may not have affected the part). Accept the feature that resulted, or use Edit Sketch or Edit Feature to change the feature definition.
I could have explained that, but the tutorials get a bit too long. As I build up some tutorial stock, I will be able to just link to explanations like that so that the flow of the tutorial is not constantly interrupted. I have an auto-link program in place that will link specific text to do just that, I just don’t have all the pieces together yet.
Hope that helps,
Mark
Hi Mark,
I'm having some trouble in this part of the tutorial. I read through some of the comments above to see if anyone had similar trouble but I don't think they did.
Right after I make my first solid tenon and apron (on the front)–the solid lines which created the top view of the tenons and aprons disappear and I'm left with only a construction line for my apron on the left. The other tenon on the left stays solid–I can still make a solid out of that. Hence, when I go to extrude the left apron–it won't let me grab it to perform the extrusion. I think the construction lines are from a previous step–so I know where they came from. I just don't know why my solid lines defining the apron (which would let me accept them to peform the apron extrusion on the left) are disappearing.
Chris
Hi Chris,
Inventor automatically consumes sketch geometry upon creation of a feature –basically, Inventor puts the sketch within the feature’s folder, and shuts off its visibility. I don’t think this should have happened, but that appears to be the case. All you need to do is expand the feature, right click on the grayed-out sketch, and choose ‘Share’ —-or, if your sketch name is present outside of a feature, but is just grayed-out, right click it and choose Visible.
You can use a sketch as many times as you wish –it just needs to be visible. Hope that helps. Good luck,
Mark