Part of my problem in learning Inventor is learning "How to think in Inventor". Maybe someone can tell me the right way to do this.
What I have is a sketch of a hole. The hole has a flattened side to prevent the part from rotating. What I want to be able to do is to put this "part" (an ipt file with just the sketch in it) on any surface of any case, top, left, right, bottom, or even the front or back. So it needs to rotate 90 degrees in x, y or z or combination thereof.
I've been told several things by the local assistants, such as "copy it, place it on the desired plane in the .ipt file, delete the original sketch, then insert it into the assembly", which doesn't work, or use the Component>Rotate command, which gives me infinite degrees of freedom, making it hard to tell when I've rotated 90 degrees in the correct axis.
The sketch will be used in a number of assemblies, including machined aluminum, 3D printing, and laser-cut acrylic.
In essence, I want to place this sketch flat on a surface, then extrude "To" the other side of the surface. I want the flat edge of this sketch (the side that keeps the part that will be inserted in the hole from rotating) constrained to be parallel to one of the edges. I have looked around a lot through the documentation and several other Web sites, and there does not seem to be an answer to this.
The sketch is simple: a circle with a flattened side, so if that sketch needs to be discarded, it is no major "expense" to me in effort. But given my projected series of projects, creating reusable drawings is going to be important. So how should I be thinking of this?
thank you
joe newcomer
Solved! Go to Solution.
Solved by PaulMunford. Go to Solution.
Solved by newcomer. Go to Solution.
I have included a trivial project to illustrate what I am trying to do. part1.ipt is a simple extruded block. part2.ipt is the outline of the hole. assembly1.iam shows what happens when I Place the two parts. Now, what I want to do is rotate part2 90 degrees counterclockwise on the Z-axis, then place it flush against the surface that is facing it. Then extrude a cut through to the other side of the surface. These are Inventor 2014 files.
Any suggestions about the way to proceed here would be appreciated. I keep finding almost-but-not-quite-related tutorials that don't help.
thanks
joe
OK, I have never looked at "iFeatures", so I will explore that. I tried a derived part and did not have much luck, but I can try again.
joe
OK, I tried a few things. I tried creating a derived part, starting with the case, which has no holes for the connectors/switches/etc. After much struggling and conferring among the Techshop staff, we were able to successfully add a hole in by creating a 2D sketch on the side of the case that would have the hole, copying the sketch (that is, Ctrl+C copy) from the hole-part, and pasting it into the sketch in the case-drawing. OK, fine, but the correlation of dimensions with the original part was lost. So I went in and used Parameter/Link to link the three parameters describing the hole to the original sketch.
Next, came the very complex connector, with the orientation cut, the odd layouts, the chamfers that describe the shape of the connector, and so on. Copy/Paste/Link is going to be a royal pain, because there are over thirty parameters that describe this hole.
So I tried to derive from the part file that contained the sketch of the holes. There is only one sketch in the file. It comes in, but it attaches itself strangely to the base drawing and refuses to be moved.
Now, the problem is that this cannot be a 3D part, because until the sketch is placed on a case and extruded through the wall, it has no 3D-reality. I can't extrude a "cut" extrusion unless I have a 3D part to extrude through. I have many different connectors, with various polarization key mechanisms in my "personal library" of parts (in my head), and I see no way to convert these various sockets, connectors, etc. into reusable part drawings.
Based on these sketches, I can create representatives of the actual parts, and my goal is to assemble the "products" so I don't end up in the fixes I found myself in thirty years ago, when I could have parts that needed to occupy the same space at the same time. But everything is parameterized like crazy, so minor changes in one drawing reflect through all the derived parts and the assemblies. Seems like a great idea, if only I could get it to work.
joe
Joe,
This should be done at the part level, not at the assembly level...unless I am missing something.
What Paul said to do above is to insert a "derived sketch Block". If you derive in the sketch from your "part2" into "Part1", you are correct in that you will not be able to move it. The sketch will be fixed in the same location in part1 as it is in part2.
Attached below is your part1, but I derived into it a sketch block from part2. Once this sketch block is created, it can be derived into as many parts that you want. You can have this sketch block in 100's of parts and if you change the dimensions of in the one sketch block file that is in Part2, then ALL the parts will be updated when they are reopened in Inventor. This might be a bad thing, depending on how you operate.
If you need to know how to create a sketch block, you can find that in Help. But basically when you are in a sketch, just click on the "Create Sketch Block" in the layout panel. After it is created, you derive just the sketch block into the part and place is into a sketch. You then use dimensions to get the sketch block placed and extrude it to make the cut.
Kirk
Thank you. I did not understand that a "sketch block" is different from a "sketch". I will try that shortly and report what happens, but it sounds like my confusion has been cleared up. Much thanks.
joe
Well, there is some progress. I can now derive a part into an assembly, and move it around. But when I try to extrude it, I get the message "No visible unadaptive sketches". This is less than informative, because if I put "unadaptive" into the Inventor search I get only two articles, neither of which seems relevant (for example, there is no "unshare" menu item). A bit of mousing around produces a right-click menu that has the word "Adaptive" in it, and there is no check mark next to "Adaptive". So while I can place the sketch blocks into an assembly, and move them to the surface where they will be extruded into mounting holes, I can't actually do the extrusion.
So, at least one problem is solved; but it has only uncovered another incomprehensible problem (an hour of reading help files and having the experts at Techshop kibbitz over my shoulder and/or push me aside while they fiddled has not produced any solution to the new problem...so it's not like I just hit a problem and posted a response without trying to at least understand what is going on. But I feel like one of the three blind men next to an elephant)
joe
.... I can now derive a part into an assembly, and move it around. But when I try to extrude it, I get the message "No visible unadaptive sketches".....
Joe, Just to get terminology correct, you can't derive a part into an assembly. You can place the part into the assembly. You can only derive a part (or assembly) into another part. Did you look at my part1 KA.ipt that I posted in message 6 above? Inside this part is a derived SKETCH BLOCK. This Sketch block is derived from Part2 KA.ipt.
When you see "No visible unadaptive sketches", it is because there is no sketch to extrude, revolve or whatever. If you have a sketch in your part that you want to use, and it maybe is already consumed by another feature, you will have to "share" the sketch (Right ckick on the sketch for a context menu). When you first make a sketch and then extrude a shape using that sketch, the visibility is turned off. To use that same sketch again, you have to share the sketch.
When you have a problem like this, either post a screen shot of what you are seeing or post the part (if possible). Not that we dont know what the error message is you are seeing, but it helps explain it if we know what you are looking at. Any long time Inventor user has seen this error and knows exactly what to do about it.
You dont want your sketches to be adaptive. Checking that will not do any good at this point.
Kirk
I am now more confused than ever.
I have not been able to reproduce the drawing examples you posted, starting from scratch. My attempts seem to be the same, but do not work the same. Note that I'm stuck using Inventor 2013 at Techshop, but I cannot reproduce them in Inventor 2014. There is some elementary concept I am missing here, and what is frustrating is that I don't even know the right questions to ask to resolve the problem. Are there any good online tutorials that would cover this? I don't mind spending time watching these, but none of the ones I've found thus far seem to address this problem.
Alas, none of the people at Techshop have a clue as to how to do this, either.
joe
Well, I have just spent six hours researching this topic, on top of 5 hours of lynda.com. What is annoying is that I have looked at possible causes and some were from sketches with unclosed loops or other problems; my sketch is Sketch Doctor Approved (sm). I have created a sketch block, marked it as an export, and in general appear to have done everything I inferred from the "partN KA" files that were uploaded. Again, though, I am working primarily in Inventor 2013, so some features may not be available.
I tried to use the "Pack and Go" option to save the assembly and all its pieces, but got the error message shown in the screen shot. I cannot even parse that sentence. The file that appears as the name given is exactly the file that is currently visible. So not only is it unparseable, but the semantics are, as best I can tell, completely undefined. Somewhere, maybe, there is an explanation, but the explanation should be accessible via a "Help" button on the dialog, that explains the message. Sadly, the Help page reached by clicking the "Help" button gives a description of options that I never get to see because the error message has caused the save to be aborted. But the message, its cause, and its resolution are not mentioned on the help page.
I think that "problem.zip" has all the necessary files. I hope. I have modified them in the way I thought was done in the examples that had been uploaded several messages back, but either that can't be done in 2013, or I have missed some critical aspect of what is being done.
The assembly file is "product case.iam", and it has an instance of "Adafruit 960 holes" (which I thought had been properly modified). I included a couple other "hole" files, which, again, I thought I had modified properly. Any hints would be appreciated.
I note that in prior instances of threads on this message, the answers fell into two categories: "That worked, thanks" for problems I double-checked and know I do not have (open loops in a sketch, for example), or "Never mind, I fixed it" with no revelation of what the fix was. Once I got the concept that a "sketch block" was different from a "sketch" I thought I had solved it, but no such luck.
joe
Joe, Sorry for the late response. I am not at work this week, but occasionally peek in here to see whats going on. Sorry you are having so much trouble with this.
"...I tried to use the "Pack and Go" option to save the assembly and all its pieces, but got the error message shown in the screen shot...."
The screen shot shows that your iam file is outside the workspace of the project file you are using. To avoid this, either select a different ipj file in the pack-n-go dialog or move the iam so that it is the workspace of an existing project. Projects is another discussion all in themselves. I use the "Single Project Method". You can find more about this if you google "Inventor Single project method.
".....I think that "problem.zip" has all the necessary files. I hope. I have modified them in the way I thought was done in the examples that had been uploaded several messages back, but either that can't be done in 2013, or I have missed some critical aspect of what is being done.
The assembly file is "product case.iam", and it has an instance of "Adafruit 960 holes" (which I thought had been properly modified). I included a couple other "hole" files, which, again, I thought I had modified properly. Any hints would be appreciated...."
I opened the "product case 2.iam". There is one file missing (case with no holes.ipt). It has an instance of "Adafruit 935 holes.ipt", but I dont see a Adafruit 960 holes.ipt". I dont see where you derived a sketch block into any of the parts that I can view. Hard to tell what is going on here, so I think I will post a video of how I created the part1 KA.ipt and part2 KA.ipt. Hopefully that will answer a few questions.
One thing that might be confusing you is the difference between sketches in an assembly and sketches in an part. Unlike sketches in a part, sketches in an assembly:
1. cant be shared (a gripe I have had for a looong time).
2. You cant create a sketch block in an assembly.
The video and workflow is the same between 2013 and 2014 ( I am using 2014 where I sit right now). This shows how to create a sketch block. I start with a sketch in a part. This is like the Part2 KA.ipt. http://screencast.com/t/Lz8w3pLtA
Next, In the part you want to bring this into....I start with a part with a simple extrusion and then derive in the sketch block from part2. This is like the Part1 KA.ipt that I posted a while back. http://screencast.com/t/JrevTiXCj
Kirk
I apologize for the incompleteness. Rather than risk it again, I'm sending a zipfile with all the files I'm working on in it. Many are irrelevant, but if you open the "Product case" assembly, at least all the necessary files should be there. I have not had a chance to look at project files; one crisis at a time.
(Again, the major problem is not even knowing what questions to ask, like "What's a project file?")
joe
I was able to open the "Product Case.iam". Now what are you trying to do with this? Are you trying to use the sketch in "Adafruit 936 Holes.ipt" to cut holes in the "Case with no holes.ipt"?
I will just assume that you are. Here is how to do it.
Sadly, this seems to be a 2014 feature, and is not available in 2013. I followed the script right up to the step of "right click on the 'Adafruit 936 holes' part, and there is no "Place block" option. I could give screen shots of all the steps, but that's a lot of bandwidth which may not be necessary. So I'm including just a snapshot of the menu item.
joe