I'm trying to figure out which is better, "make part" or "derive." I'm sure both have there pros and cons, and I'd like to hear what experienced users have to say. Yes I searched the forums and came up empty for such a comparison.
Thanks.
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I'm trying to figure out which is better, "make part" or "derive." I'm sure both have there pros and cons, and I'd like to hear what experienced users have to say. Yes I searched the forums and came up empty for such a comparison.
Thanks.
Neither is a "better" approach. The choice depends upon your design intent and workflow, and whether you have existing parts/assembly or are creating new parts. Derive imports data from an existing part, assembly or Alias *.wire, whereas Make Part exports data into a new part.
Suppose you have designed and completed Part A that will be a raw casting. Part A will be derived into a new Part B, which will have the machined features applied. You can use either Derive or Make Part to create the machined version:
Case 1 - Derive: Create new Part B. The Derive tool will import the Part A solid, and any additional data (parameters, surfaces, etc.) into this part. Apply the necessary machined features.
Case 2 - Make Part: Part A is open. The Make Part tool will export solids, parameters, etc. into, and create the new Part B. Apply the necessary machined features.
This is a very simple example, but in both cases, Part A is derived into and drives Part B, and the resulting parts are identical. There are many other possibilities and results.
There is also the Make Components tool which allows you to generate an assembly composed of derived parts created using a multi-body solid. Very slick. I use it alot. Anyway...
My $.02...
Thanks Bunny; the terms export and import make more sense to me than the "push/pull" verbiage others have used.
Although I've been using CAD since 1979, primarily in heavy industrial and commercial buildings and facilities, I've only been using Inventor the past couple of years on a sporadic basis for creating things I haven't done since school; so I have a lot to learn.
In my case I'm designing/replicating axles for a plastic model truck. I did the main housing first, and then I DERIVED the axle housing to create the differential carrier housing that has a common mating surface. After I completed the differential carrier housing I unsuppressed the axle housing and got the error message dialog box; so I suppressed the axle housing and went on my way.
With that in mind, when it came to creating the input shaft housing part that mates up with the differential carrier housing, I tried MAKE PART for that small piece. All went well until I discovered I had to adjust the hole locations on the bolt circle. I corrected that issue on the differential carrier housing, and the input shaft housing part went higgly-piggly. I started over on the part as it was simple instead of trying to correct whatever was making Inventor unhappy.
I don't have my graphics PC running at the moment to post some in progress screen shots.
DERIVE = import, MAKE PART = export.
Without seeing the assembly, my first thought would be to try a multi-body part and use Make Components. All of the geometry can be exported into the individual parts. Then, perhaps, you could use a bolted connection to create the bolt holes. Any chance you can post something?
Here are some in progress screen shots.
I use derive where I want there to be a relational link between the 2 parts.
So that a change in A will automatically update B (which is derived from A).
An example could be cable routing around a machine or structure. You make alterations to the housing (part A), increase the size or moving some holes, and the cable trays/cables (part B), that are have their lengths and locations constrained to the derived housing, will move, grow or shrink accordingly.
Make Part breaks any links with the parent, making it independent.
... I suppose a simpler way of putting it in old CAD language would be to say that Derive = xref and Make part = block
That is not correct...Quote:
Originally Posted by KCM
Look at Make Part Dialog.jpg. In the upper left corner, you will see "Derive Style", and directly below, all of the items available to be derived/exported from this part into the new part. Notice the Part name "Knot - Derived". Clicking OK generates the new Knot - Derived.ipt and opens it.
Knot - Derived A.jpg shows the Knot - Derived.ipt model tree
Knot - Derived B.jpg shows the Knot - Derived.ipt model tree with the flyout that displays when you RMB on the Knot.ipt entry. On this flyout, in blue, you see the option "Edit Derived Part".
If you want this part to be "independent" as you say, you have 2 options:
1. "Suppress Link With Base Component" - Any changes to the Knot.ipt so any changes will not update this part. This is a temporary suppression and can be undone at a later time.
2. "Break Link With Base Component" - Permanently removes any association to the original.
Thank you both, and the differences between the two commands and when to use them are becoming more clear to me.
I stand corrected, thank you :)Quote:
Originally Posted by Bunny