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"make part" or "derive"...which is better?

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Message 1 of 18
iMaJiNe_Designs
863 Views, 17 Replies

"make part" or "derive"...which is better?

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.

17 REPLIES 17
Message 2 of 18
BeKirra
in reply to: iMaJiNe_Designs

IMO, "Make Part" is different to "Derive".

Both "Make Part" and "Derive" works in an IPT enviroment.

The difference is that "Make Part" exports features (Solid, Surface Bodies,Blocks, Sketches, 3D Sketches, Work Geometry, iMates or Parameters) from the IPT while "Derive" imports IPT or IAM to the current IPT.

 

I would also like to hear what the experienced guys says.

Please mark "Accept as Solution" and "Like" if my reply resolves the issue and it will help when others need helps.
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Message 3 of 18
admaiora
in reply to: BeKirra

There is no better. Simply they are tools, that technically works similar, but that have different tasks.

 

es1: i am working in multibody and i want to create only  a part from a body >> Make Part

 

es2: i need to start a new part  and i need references from a part that i have already modelled >> Derive

Admaiora
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Message 4 of 18
iMaJiNe_Designs
in reply to: admaiora

Thank you both for your quick replies.

 

@admaiora:  By multibody; do you mean a single part file with multiple solids listed in the model browser, or do you mean an assembly?

 

Is there a way to convert from "make part" to "derive" and vice-versa, or is that on the Inventor wish list?

 

Thanks again.

Message 5 of 18
admaiora
in reply to: iMaJiNe_Designs

Yes, multibody= part  with multiple solid bodies inside

 

No, one derives, and the other makes a part.

Admaiora
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Message 6 of 18
JDMather
in reply to: iMaJiNe_Designs

They do the same thing.

One pushes out the geometry.

The other pulls in the geometry.

 

The initial result is identical.

Derive has a bit more functionality pulling in geometry. (assembly...


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Message 7 of 18
iMaJiNe_Designs
in reply to: JDMather

Thanks for your input.  I'm no Inventor expert; but I know enough to be dangerous so to speak.

 

In any case I need to experiment with both commands further.

 

I'm working on rear axles for a plastic model truck, and I built the main axle housing as one part.  Then I used DERIVE to start the differential carrier part so I could obtain the axle housing to differential carrier mounting flange and bolt circle.  This worked well; but when I went to unsuppress the axle housing in the derived part I got all sorts of error messages, so I'm leaving the axle housing suppressed.

 

Then I decided to try MAKE PART when I needed to make the input shaft cover that attaches to the reduction gear cover on the differential carrier.  This is when I discovered I had to adjust the bolt circle.  I changed the bolt circle on the reduction gear cover successfully; but the input cover created with the MAKE PART command went higgly piggly, and I had to essentially start over on the input shaft cover.  Fortunately it's a simple part.

 

In both cases I did not automatically place the parts in an assembly.  I will make the assembly file later.

Message 8 of 18

I'm glad someone started this thread. It has been most helpful. 

 

@iMaJiNe_Designs if your models have issues updating then perhaps you should look at best practices in terms of building your model as in fully constraining it, how you build your references and making sure you don't create any rebuild loops. 

 

I find it helpful using mostly planes and axis for my sketches, all linked with parameters to the Origin. If you start snapping or constraining to solid bodies which can potentially update in your model, you lose references or create loops and that's when issues come up. 

 

 

Message 9 of 18
IgorMir
in reply to: iMaJiNe_Designs

Hi Matthew,

As it has already been mentioned - it is not a question of "which is better" but rather - when and where to use different tools.

There was a topic the other day about mismatch flanges width in sheet metal module. I  prefer to use Derive components workflow when creating models. But this time around multi-solid approach was a better choice. Since to establish a relationship between corresponding flanges and create individual components was more straightforward using multi-solid environment.
Attached is an example of multi-solid  part in IV2020 format.

Cheers,
Igor.


@iMaJiNe_Designs wrote:

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.


Web: www.meqc.com.au
Message 10 of 18
BDCollett
in reply to: iMaJiNe_Designs

I am going to assume that user has likely learned quite a lot in the 7 years since they made this post.

Message 11 of 18
iMaJiNe_Designs
in reply to: BDCollett

Time flies!

Message 12 of 18
Totka.Ivanova
in reply to: BDCollett

I've started using one master multibody part for complex joinery or metalwork(because it's easier to have a couple of shared sketches then dozens) which I then use to both "make part" and "derive" part from. The derived one I use in my large assemblies, and the assembly made from "make part" I use for the CNC drawings of the separate panels/parts which I've automated with the AutoDraw AddIn. I'm happy with this workflow. Updates fairly quickly from the external parameter table, even though my computer is not the most powerful.

 

@BDCollett  My presumption is that the posts on this forum are for all users to learn from, not just the person posting the initial question?

 

 

Message 13 of 18
SBix26
in reply to: Totka.Ivanova

One thing that I'm not sure has been explicitly stated in this thread: Derive and Make Part (Make Components) are two different workflows for doing the exact same thing.  Make Part & Make Components are simply convenient wizards to produce derived parts.  The end result is the same thing, derived parts.

 

As @JDMather pointed out (several years ago!), using the Derive tool from the "receiving" end of the process has more options available to tweak the process, but that does not change the fact that using Make Part creates a derived part.  In fact, if you then edit that newly created part, you will see a Derive feature in the model browser, and you can edit that Derive feature as needed, exactly the same as if you had manually created that Derive feature yourself.

 

For myself, I typically use Derive as I'm working on a design so that I explicitly consider which .ipt template I wish to use, and to assign materials/appearances and iProperties at the time of creation.  I then add the new part to the assembly, so I can clearly see how the final product is developing as the design progresses.

 

Hope that clarifies things,


Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
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Message 14 of 18

Hi Folks,

 

The two commands are for two different purposes. The traditional Derive offers atomic control to individual derivable objects in a given source. Make Part and Make Components are meant to supplement Multi-Solid Body Push Derive workflows. Basically, you define the geometry of an assembly as a multi-solid body part. Then you need to push individual solid body as a real part to proceed with assembly-level design workflows (constraints, BOM, and so on).

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 15 of 18

@johnsonshiue thank you for this.

 

When I was reading the Large Assembly Modeling Workflows on the official Autodesk inventor support page, there is quite a lot of mention of derived parts and how they should be used, not so much about the Make Part command we can use for our Multi bodies. 

 

So I have a question in terms of enhancing the performance of my large assemblies:

1) With a derived multibody we can scale, mirror, supress/unsupress, convert to surfaces etc etc. 

2) With a "make part" multibody we can only supress/unsupress features.

 

So let's say the sole purpose is making the large assembly load faster and we are not editing anything else in our multibody parts we will be placing in it. 

 

Which one is faster? 1) or 2)?

 

Thanks!

Message 16 of 18

Hi! If you are talking about large assembly design, I don't believe multi-solid body workflow should be in the equation. If you have to use it, you want to limit the usage. Here is a very simple example to illustrate my point.

Think of 1000 boxes. If you model them as multi-solid bodies in a part, you will need 1000 bodies. The part will be relatively heavy. Then you push each body as a part in an assembly. You will get 1000 unique parts (files) in the assembly, which is also heavy.

If you model a box as a part, you can easily create 1000 instances within an assembly. It will be very compact. You only need an iam file and an ipt file representing the whole thing.

Inventor is a distributed design CAD system. It thrives on distributing geometry among parts and reusing the same part definition. Most of the machinery design is like this. It is very rare you have all 1000 unique parts. It will be very expensive to make.

Multi-solid body workflow is meant for smaller assembly with mostly unique parts. Things like mouses or coffee machines. The parts are mostly unique and they have spatial dependency.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 17 of 18

Thank you @johnsonshiue.

 

How many unique parts in an assembly makes a “small” assembly transition to a “large” one? 100? 500? 

Message 18 of 18

Hi! It is hard to say. It would depend on the geometric complexity. Like the box example I mentioned earlier, 10000 unique boxes should be fine.

At the moment, I have seen our users building assembly with 500K components with 10K unique components. So, 100 or 500 is trivial.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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